anilam 3000 User Manual

Download

3000M CNC

Programming and Operations

Manual for

Three- and Four-Axis Systems

www.anilam.com

CNC Programming and Operations Manual

P/N 70000504I - Contents

Section 1 - CNC Programming Concepts

Programs .......................................................................................................................................... 1-1

Axis Descriptions .............................................................................................................................. 1-1

X Axis ........................................................................................................................................... 1-2

Y Axis ........................................................................................................................................... 1-2

Z Axis ........................................................................................................................................... 1-2

Defining Positions ............................................................................................................................ 1-2

Polar Coordinates ......................................................................................................................... 1-3

Absolute Positioning ..................................................................................................................... 1-3

Incremental Positioning ................................................................................................................ 1-4

Tool-Length Offsets .......................................................................................................................... 1-5

Tool Diameter Compensation ........................................................................................................... 1-6

Using Tool Diameter Compensation and Length Offsets with Ball-End Mills ................................. 1-10

Angle Measurement ....................................................................................................................... 1-10

Corner Rounding ............................................................................................................................ 1-11

Line-to-Line Corner Rounding .................................................................................................... 1-11

Line-to-Arc Corner Rounding ...................................................................................................... 1-12

Arc-to-Arc Corner Rounding ....................................................................................................... 1-12

Chamfering ..................................................................................................................................... 1-13

Plane Selection .............................................................................................................................. 1-14

Arc Direction ................................................................................................................................... 1-15

Section 2 - CNC Console and Software Basics

Console ............................................................................................................................................ 2-1

Keypad ............................................................................................................................................. 2-1

Programming Hot Keys ................................................................................................................ 2-2

Editing Keys ................................................................................................................................. 2-3

Manual Operation Keys ................................................................................................................ 2-3

Operator Keys .............................................................................................................................. 2-4

Soft Keys (F1) to (F10) ..................................................................................................................... 2-5

Off-line Keyboard (Optional) ............................................................................................................. 2-5

Software Basics ............................................................................................................................... 2-5

Pop-up Menus .............................................................................................................................. 2-5

Screen Saver ................................................................................................................................ 2-6

Switching Selections with the Toggle Key .................................................................................... 2-6

Clear Key ...................................................................................................................................... 2-6

Operator Prompts ......................................................................................................................... 2-6

ASCII Chart .................................................................................................................................. 2-6

Cursor and Highlight Functions .................................................................................................... 2-7

Entering Text ................................................................................................................................ 2-7

Typing Over and Inserting Letters and Numbers .......................................................................... 2-7

Deleting Characters ...................................................................................................................... 2-8

Messages/Error Messages ............................................................................................................... 2-8

Section 3 - Manual Operation and Machine Setup

Powering On the CNC ...................................................................................................................... 3-1

Shutting Down the CNC ................................................................................................................... 3-1

Emergency Stop (E-STOP) ................................................................................................................ 3-1

Performing an Emergency Stop ....................................................................................................... 3-1

Activating/Resetting the Servos ....................................................................................................... 3-2

(Re-)Starting the Spindle .................................................................................................................. 3-2

CNC Programming and Operations Manual

P/N 70000504I - Contents

Manual Mode Screen ....................................................................................................................... 3-3

Primary Display Area Labels ........................................................................................................ 3-4

Secondary Display Area Labels .................................................................................................... 3-4

Position Display ............................................................................................................................ 3-5

Manual Machine Operation .............................................................................................................. 3-6

Manual Mode ................................................................................................................................ 3-6

Auto Mode .................................................................................................................................... 3-6

Mode Settings .................................................................................................................................. 3-7

Activating Manual Mode Rapid or Feed ........................................................................................... 3-8

Setting a Feedrate ........................................................................................................................ 3-8

Adjusting Rapid Move Speed ....................................................................................................... 3-8

Overriding the Programmed Spindle RPM.................................................................................... 3-9

Absolute/Incremental Modes ........................................................................................................ 3-9

Inch/MM Modes ............................................................................................................................ 3-9

Setting Absolute Zero ................................................................................................................. 3-10

Defining Absolute Zero in X and Y Axes ..................................................................................... 3-10

Presetting the X- or Y-Axis ......................................................................................................... 3-10

Fixture Offsets (Work Coordinate System) ................................................................................. 3-11

Setting Tool Change Position ..................................................................................................... 3-12

Locating Tool #0, Z0 ................................................................................................................... 3-12

Presetting the Z-Axis .................................................................................................................. 3-13

Activating a Tool ......................................................................................................................... 3-13

Activating a Plane ....................................................................................................................... 3-13

Activating a Spindle RPM (Requires Programmable Spindle Option) ......................................... 3-14

Jog Moves ...................................................................................................................................... 3-14

Changing the Jog Mode ............................................................................................................. 3-15

Jogging the Machine (Conventional) .......................................................................................... 3 -15

Jogging the Machine (Continuous) ............................................................................................. 3-16

Operating the Handwheel (Optional) .............................................................................................. 3-16

One-Shot Moves ............................................................................................................................ 3-17

Manual Data Input .......................................................................................................................... 3-17

Disengaging the Z-Axis Drive System ............................................................................................ 3-19

Section 4 - Writing Programs

Program Basics ................................................................................................................................ 4-1

Developing Part Programs ............................................................................................................... 4-1

Writing Program Blocks .................................................................................................................... 4-3

Using Graphic Menus ................................................................................................................... 4-3

No Move Blocks ............................................................................................................................... 4-4

Programming an Absolute/Incremental Mode Change ................................................................. 4-4

Programming an Inch/MM Mode Change ..................................................................................... 4-4

Programming a Tool Change ........................................................................................................ 4-5

Activating a Tool ........................................................................................................................... 4-5

Activating Tool-Diameter Compensation ...................................................................................... 4- 6

Programming a Dwell ................................................................................................................... 4-7

Programming a Return to Machine Zero ...................................................................................... 4-8

Programming Fixture Offsets ........................................................................................................ 4-9

Resetting Absolute Zero (Part Zero) ........................................................................................... 4-11

Programming a Plane Change ................................................................................................... 4-13

Programming a Feedrate Change .............................................................................................. 4-14

Programming a Spindle RPM ..................................................................................................... 4-15

CNC Programming and Operations Manual

P/N 70000504I - Contents

Straight Moves ............................................................................................................................... 4-16

Programming a Rapid Move ....................................................................................................... 4-16

Programming a Line Move.......................................................................................................... 4-17

Programming a Modal Move ....................................................................................................... 4-17

Teach Mode (Programming from the Part) ..................................................................................... 4-18

Line or Rapid Moves ...................................................................................................................... 4-19

Programming a Move Using XY Location, Radii, or Angles ........................................................ 4-20

Arcs ................................................................................................................................................ 4-21

Selecting the Plane for an Arc .................................................................................................... 4-21

Programming an Arc Using an Endpoint and Radius ................................................................. 4-21

Programming an Arc Using the Center and Endpoint ................................................................. 4-23

Programming an Arc Using the Center and the Included Angle ................................................. 4-25

Programming M-Code Blocks ........................................................................................................ 4-27

Dry Run M-Codes ....................................................................................................................... 4-28

U-Axis Synchronization M-Codes ............................................................................................... 4-28

Section 5 - Programming Canned Cycles, Ellipses, and Spirals

Drilling Cycles .................................................................................................................................. 5-1

Basic Drill Cycle ............................................................................................................................ 5-2

Peck Drilling Cycle ........................................................................................................................ 5-3

Boring Cycle ................................................................................................................................. 5-4

Chip Break Cycle .......................................................................................................................... 5-5

Tapping Cycle ............................................................................................................................... 5-7

Drill Pattern ................................................................................................................................... 5-8

Bolt Hole Pattern .......................................................................................................................... 5-9

Thread Milling Cycle ................................................................................................................... 5-11

Pocket Cycles ................................................................................................................................ 5-16

Facing Cycle ............................................................................................................................... 5-17

Rectangular Profile Cycle ........................................................................................................... 5-19

Circular Profile Cycle .................................................................................................................. 5-21

Rectangular Pocket Cycle .......................................................................................................... 5-23

Circular Pocket Cycle ................................................................................................................. 5-25

Frame Pocket Cycle ................................................................................................................... 5-27

Hole - Mill Cycle .......................................................................................................................... 5-29

Irregular Pocket Cycle ................................................................................................................ 5-31

Pockets with Islands ................................................................................................................... 5-36

Subprograms .................................................................................................................................. 5-39

Situation: 1 (Repetitive Drilling Cycle) ........................................................................................ 5-39

Situation: 2 (Rough and Finish Cycles) ...................................................................................... 5-39

Subprogram Structure ................................................................................................................ 5-39

Subprogram Example ................................................................................................................. 5-39

Organizing Programs Containing Subprograms ......................................................................... 5-40

Calling Subprograms from the Main Program ............................................................................. 5-40

Ending Main Programs ............................................................................................................... 5-40

Starting Subprograms ................................................................................................................. 5-41

Ending Subprograms .................................................................................................................. 5-41

Looping Subprograms ................................................................................................................ 5-41

Rotating, Mirroring, and Scaling Subprograms (RMS) ................................................................ 5-42

Ellipses and Spirals ........................................................................................................................ 5-43

Plane Selection ........................................................................................................................... 5-43

Programming an Ellipse ............................................................................................................. 5-43

Programming a Spiral ................................................................................................................. 5-45

CNC Programming and Operations Manual

P/N 70000504I - Contents

Mold Cycles .................................................................................................................................... 5-47

Programming a Mold Rotation .................................................................................................... 5-47

Rotations Around X- and Y- Axes (Small Radius) ...................................................................... 5-48

Rotations Around X- and Y- Axes (Large Radius) ...................................................................... 5-52

Rotation Around the Z-Axis ........................................................................................................ 5-53

Programming an Elbow Milling Cycle ......................................................................................... 5-55

Engraving, Repeat, and Mill Cycles ............................................................................................... 5-60

Engraving Cycle ......................................................................................................................... 5-60

Repeat Cycle .............................................................................................................................. 5-62

Mill Cycle .................................................................................................................................... 5-64

Probing Cycles ............................................................................................................................... 5-66

Tool Probe Cycles ...................................................................................................................... 5-66

Spindle Probe Cycles ................................................................................................................. 5-83

Section 6 - Editing Programs

Activating the Program Editor ........................................................................................................... 6-1

The Program Editor Screen .............................................................................................................. 6-2

Saving Edits ..................................................................................................................................... 6-3

Canceling Unsaved Edits ................................................................................................................. 6-3

Deleting a Program Block ................................................................................................................. 6-3

Inserting a Program Block ................................................................................................................ 6-4

Editing a Program Block ................................................................................................................... 6-4

Searching Blocks for Words or Numbers ...................................................................................... 6-4

Scrolling the Program Listing ........................................................................................................ 6-4

Paging through the Program Listing ............................................................................................. 6-5

Jumping to First or Last Block in the Program .............................................................................. 6-5

Using Comments .............................................................................................................................. 6-5

Writing a Comment Block ............................................................................................................. 6-5

Commenting Out Existing Blocks ................................................................................................. 6-5

Canceling a Comment .................................................................................................................. 6-6

Using Block Operations to Edit a Program ....................................................................................... 6-6

Section 7 - Viewing Programs with Draw

Draw Modes ..................................................................................................................................... 7-1

Starting Draw ................................................................................................................................... 7-2

Draw Screen Description .................................................................................................................. 7-3

Putting Draw in Hold ........................................................................................................................ 7-3

Canceling Draw ................................................................................................................................ 7-3

Draw Parameters ............................................................................................................................. 7-4

Text On or Off ............................................................................................................................... 7-4

Tool On or Off ............................................................................................................................... 7-5

Drawing Compensated Moves ...................................................................................................... 7-5

Showing Rapid Moves .................................................................................................................. 7-6

Setting Grid Line Type .................................................................................................................. 7-6

Setting Grid Size ........................................................................................................................... 7-6

Putting Draw in Motion, Single-Step, or Auto Mode ...................................................................... 7-7

Automatic Draw Restart ................................................................................................................ 7-8

Erasing Display ............................................................................................................................. 7-8

Running Draw for Selected Blocks ............................................................................................... 7-8

Adjusting Draw Display .................................................................................................................. 7-10

Fitting the Display to the Viewing Window .................................................................................. 7-10

Halving Display Size ................................................................................................................... 7-10

Doubling Display Size ................................................................................................................. 7-10

CNC Programming and Operations Manual

P/N 70000504I - Contents

Scaling the Display by a Factor .................................................................................................. 7-11

Zooming In ................................................................................................................................. 7-11

Erasing Display ........................................................................................................................... 7-11

Changing Draw Views ................................................................................................................ 7-12

Selecting the View ...................................................................................................................... 7-12

Section 8 - Running Programs

Selecting Programs for Running ...................................................................................................... 8-1

Running a Program One Step at a Time .......................................................................................... 8-1

Single-Step Mode vs. Motion Mode .............................................................................................. 8-2

Holding or Canceling a Single-Step Run ...................................................................................... 8 -2

Single-Step Execution of Selected Program Blocks ..................................................................... 8-2

Switching from Single-Step to Auto .............................................................................................. 8-3

Auto Program Execution .................................................................................................................. 8-3

Holding or Canceling an Auto Run ............................................................................................... 8-3

Starting at a Specific Block ........................................................................................................... 8-4

Clearing a Halted Program ............................................................................................................... 8-4

Using Draw while Running Programs ............................................................................................... 8-5

Parts Counter and Program Timer ................................................................................................... 8-6

Background Mode ............................................................................................................................ 8-7

Section 9 - Program Management

Program Directory ............................................................................................................................ 9-1

Changing the Program Directory Display ......................................................................................... 9-2

Creating a New Program .................................................................................................................. 9-2

Choosing Program Names ............................................................................................................... 9-2

Loading a Program for Running ....................................................................................................... 9-2

Selecting a Program for Editing and Utilities .................................................................................... 9-3

Maximizing Program Storage Space ................................................................................................ 9-3

Program File Utilities ........................................................................................................................ 9-3

Displaying Program Blocks (Listing a Program) ........................................................................... 9-4

Deleting a Program ....................................................................................................................... 9-4

Reading Disks in Floppy Drives (Logging to Other Drives) ........................................................... 9-4

Marking and Unmarking Programs ............................................................................................... 9-5

Deleting Groups of Programs ....................................................................................................... 9-6

Restoring Programs ...................................................................................................................... 9-6

Copying Programs to Floppy Disks .............................................................................................. 9-6

Renaming Programs ..................................................................................................................... 9-7

Printing Programs ......................................................................................................................... 9-7

Formatting Floppy Disks ............................................................................................................... 9-7

Converting G-Code Programs to CNC Conversational Format .................................................... 9-8

Checking Disks for Lost Data ......................................................................................................... 9-14

Displaying System Information ....................................................................................................... 9-15

Copying Programs from/to Unspecified Locations ......................................................................... 9-16

Renaming Programs from/to Unspecified Locations ...................................................................... 9-16

Printing from Floppy Drives ............................................................................................................ 9-17

Section 10 - Tool Management

Tool Page ....................................................................................................................................... 10-1

Entering the Tool Page................................................................................................................... 10-1

Tool Page Description .................................................................................................................... 10-2

CNC Programming and Operations Manual

P/N 70000504I - Contents

Using the Tool Page ....................................................................................................................... 10-3

Finding Tools by Number ........................................................................................................... 10-3

Changing Tool Page Values ....................................................................................................... 10-3

Clearing a Tool (Whole Row) ...................................................................................................... 10-4

Clearing a Single Value .............................................................................................................. 10-4

Adjusting a Single Value ............................................................................................................. 10-4

Setting Tool-Length Offset .......................................................................................................... 10-4

Automatically Setting Tool-Length Offsets from the Tool Page .................................................. 10-5

Manually Setting Tool-Length Offsets from the Tool Page ......................................................... 10-5

Setting Tool-Length Offset for Ball-End Mills .............................................................................. 10-5

Fixture Offsets ............................................................................................................................ 10-5

Setting RefProg Offset ................................................................................................................ 10-6

Section 11 - Communication and DNC

Communication .............................................................................................................................. 11-1

Installing the RS-232 Cable ............................................................................................................ 11-1

Accessing the Communication Package ........................................................................................ 11-2

Setting Communication Parameters ............................................................................................... 11-3

Selecting the Communication Port ............................................................................................. 11-3

Setting the Baud Rate ................................................................................................................ 11-4

Setting Parity .............................................................................................................................. 11-4

Setting Data Bits ......................................................................................................................... 11-4

Setting Stop Bits ......................................................................................................................... 11-4

Software Settings ....................................................................................................................... 11-4

Setting Data Type ....................................................................................................................... 11-4

Testing the Data Link ..................................................................................................................... 11-4

Activating the Test Link Screen ...................................................................................................... 11-5

Setting Test Link Display Modes ................................................................................................ 11-5

Testing the Link .......................................................................................................................... 11-6

Clearing the Receive Area .......................................................................................................... 11-6

Sending a Program ........................................................................................................................ 11-6

Receiving a Program ...................................................................................................................... 11-7

Setting the Transmission and Receiving Display ........................................................................ 11-7

Holding Transmission/Receiving Operations .............................................................................. 11-7

Running in DNC ............................................................................................................................. 11-8

Using Data Control (DC) Codes ..................................................................................................... 11-9

Using DC Codes In Receive Mode ........................................................................................... 11-10

Using DC Codes In Send Mode ................................................................................................ 11-10

Section 12 - Calculators

CNC Calculator Package ............................................................................................................... 12-1

Math Calculator .............................................................................................................................. 12-1

Math Calculator Basics ............................................................................................................... 12-2

Operations Involving Two Numbers ............................................................................................ 12-3

Math with a Column of Numbers ................................................................................................ 12-3

Using Parentheses ..................................................................................................................... 12-3

Using Additional Functions ......................................................................................................... 12-4

Storing Numbers from the Math Calculator ................................................................................ 12-5

Right Triangle Calculator ................................................................................................................ 12-5

Activating the Triangle Calculator ............................................................................................... 12-5

Using the Triangle Calculator ..................................................................................................... 12-6

Storing Right Triangle Calculator Results ................................................................................... 12-6

Hiding the Right Triangle Calculator Screen ............................................................................... 12-6

CNC Programming and Operations Manual

P/N 70000504I - Contents

Geometry Calculator ...................................................................................................................... 12-7

Activating the Geometry Calculator ............................................................................................ 12-7

Geometry Calculator Screen ...................................................................................................... 12-7

Using the Geometry Calculator ................................................................................................... 12-8

Point Templates .......................................................................................................................... 12-9

Line Templates ......................................................................................................................... 12-10

Circle Templates ....................................................................................................................... 12-11

Deleting Selected Elements ..................................................................................................... 12-11

Deleting All Elements ............................................................................................................... 12-11

Listing All Geometry Elements ................................................................................................. 12-12

Calculating the Distance between Two Elements ..................................................................... 12-12

Last Position Recall .................................................................................................................. 12-12

Recalling Values into a Program .................................................................................................. 12-13

Recalling Values from the Math Calculator ............................................................................... 12-13

Recalling Values from the Right Triangle Calculator ................................................................ 12-14

Recalling Values from the Geometry Calculator ....................................................................... 12-15

Recalling Values from One Calculator into Another .................................................................. 12-15

Section 13 - Off-line Software

Passwords ...................................................................................................................................... 13-1

Exiting the Software ....................................................................................................................... 13-1

Windows Installation (Use Windows Installation Disk) ................................................................... 13-1

Running from Windows .............................................................................................................. 13-2

Setting up the Icon ...................................................................................................................... 13-2

System Settings ............................................................................................................................. 13-3

Maximum Memory Allocated ...................................................................................................... 13-3

Disabled Features ...................................................................................................................... 13-3

Using Soft Keys from a Keyboard .................................................................................................. 13-4

Keypad Equivalent Keyboard Keys ................................................................................................ 13-4

Editing with a Text Editor................................................................................................................ 13-7

Section 14 - Four-Axis Programming

Axis Types ...................................................................................................................................... 14-1

Rotary Axis Programming Conventions .......................................................................................... 14-2

Non-Synchronous or Synchronous Auxiliary Axis .......................................................................... 14-2

Programming Examples ................................................................................................................. 14-3

Example 1: Drill (Sync-Off) ........................................................................................................ 14-3

Example 2: Mill (Sync-On) ......................................................................................................... 14-5

Example 3: Mill (Sync-On) ......................................................................................................... 14-6

Section 15 - DXF Converter Feature

Requirements ................................................................................................................................. 15-1

Off-line Software ......................................................................................................................... 15-1

Machine Software ....................................................................................................................... 15-1

Entry to the DXF Converter ............................................................................................................ 15-2

Creating Shapes ......................................................................................................................... 15-2

Contours ..................................................................................................................................... 15-3

Drilling ........................................................................................................................................ 15-3

CNC Code ...................................................................................................................................... 15-3

Mouse Operations .......................................................................................................................... 15-4

DXF Hot Keys ................................................................................................................................ 15-5

Toggle Entity Endpoints (ALT + F) ............................................................................................. 15-5

CNC Programming and Operations Manual

P/N 70000504I - Contents

DXF Soft Keys ................................................................................................................................ 15-6

Miscellaneous DXF Soft Key, F6 ................................................................................................ 15-7

Output Menu Options ..................................................................................................................... 15-8

Shift X, Shift Y Descriptions ........................................................................................................ 15-8

Convert Polyline Description ....................................................................................................... 15-9

Display Menu Options .................................................................................................................... 15-9

DXF Entities Supported ................................................................................................................ 15-10

Drawing Entities Not Supported ................................................................................................ 15-10

Files Created ................................................................................................................................ 15-11

DXF Example ............................................................................................................................... 15-11

Unedited Conversational Program Listing ................................................................................ 15-13

Edited Conversational Tool Path .............................................................................................. 15-14

Edited Conversational Program Listing .................................................................................... 15-14

Using DXF for Pockets with Islands.......................................................................................... 15-16

Section 16 - CNC Software

Machine Software Installation ........................................................................................................ 16-1

Software Option Kit Installation ...................................................................................................... 16-1

Procedure ................................................................................................................................... 16-1

Using Soft Keys from a Keyboard .................................................................................................. 16-2

Keypad Equivalent Keyboard Keys ................................................................................................ 16-2

Making Jog Moves from a Keyboard .............................................................................................. 16-2

Index ....................................................................................................................................... Index-1

CNC Programming and Operations Manual

P/N 70000504I - CNC Programming Concepts

Section 1 - CNC Programming Concepts

Programs

This manual describes CNC programming and operations for 3000M three-axis systems.

A program is the set of instructions used by the CNC to direct machine movement. Each instruction is called a block and each block executes independently.

Programs are stored in the CNC’s memory and accessed from the CNC’s Program Directory. You can create, delete, copy, and rename programs in the CNC’s Program Directory.

Axis Descriptions

The machine moves along its axes of motion. All movement along an axis is in either a positive or negative direction. Not all machines use the same system for identifying axes. The descriptions here are most commonly used for three axis mills. Refer to Figure 1-1.

NOTE: To keep directions straight when programming machine

movements, consider tool motion rather than table motion. (When tool motion is positive, table motion in negative, and vice versa.)

Figure 1-1, Mill Axes of Motion (Tool Motion Orientation)

CNC Programming and Operations Manual

P/N 70000504I - CNC Programming Concepts

X Axis

The table moves left and right along the X-axis. Positive motion is table movement to the left (tool, right); negative motion is table movement to the right (tool, left).

Y Axis

The table moves in and out along the Y-axis. Positive motion is table movement out (tool, in); negative motion is table movement in (tool, out).

Z Axis

In the Z-axis, the tool moves up and down on the spindle. Positive motion is tool movement up; negative motion is tool movement down (into the work).

Defining Positions

The intersection of the X, Y, and Z-axes is the reference point that defines most positions. This point is the X0, Y0, and Z0 position. Refer to Figure 1-2.

Most positions are identified by X, Y, and Z coordinates. A position two inches left, three inches back, and four inches up has the following coordinates:

X-2.0 Y3.0 Z4.0

-2

X+

Figure 1-2, Locating Positions

CNC Programming and Operations Manual

P/N 70000504I - CNC Programming Concepts

Polar Coordinates

Polar Coordinates define points that lie on the same plane. Polar coordinates use the distance from the origin and an angle to locate points. Refer to

Figure 1-3.

POLAR

Figure 1-3, Polar Coordinate System

Absolute Positioning

In the Absolute Mode, all positions are measured from the Absolute Zero Reference point. Absolute Zero is not a fixed position on the machine, but a point you select. Refer to

You can set the Absolute Zero Reference point (X0, Y0) anywhere. Usually the Absolute Zero Reference is set at a position that makes it easy use the dimensions from the blueprint. This is also called setting the Part Zero.

Figure 1-4.

BSOLUTE

Figure 1-4, Absolute Positioning

CNC Programming and Operations Manual

P/N 70000504I - CNC Programming Concepts

Incremental Positioning

Measure incremental moves from the machine’s present position. This is convenient for performing an operation at regularly spaced intervals. Refer to

Figure 1-5.

NOTE: An incremental 0-inch/0-mm move will not make a position

change.

First increment Second increment Third increment Fourth increment

Original Location

Figure 1-5, Incremental Positioning

INCREMENTAL

CNC Programming and Operations Manual

P/N 70000504I - CNC Programming Concepts

Tool-Length Offsets

The operator sets the Z0 position of the quill, from which the CNC applies Tool-Length Offsets. Usually it is the fully retracted position of the quill.

NOTE: For machines without homing, it may be necessary to set

machine home to make setting tool-length offsets easier. Either manually or by jogging take the Z-axis close to the top of travel. The servo must be turned on. Press MDI (F7), press Mill (F5), press More (F7), curse down to Home and press ENTER, press Z the z will light up, press Save, press Prev, press Exit, and press

Start. The Z-axis will change to zero.

Because tools differ in length, Z0 axis (Part Zero) is not set the same way as X0 or Y0. The tool-length offset is the distance from the tip of the tool to the top of the part. Enter a length offset for each tool in the Tool Page. (Refer to “Section 10 - Tool Management.”)

Tool-length offset is the distance from Z0 Tool #0 to the tip of the tool at the part Z0 (usually the surface of the work). Refer to

Figure 1-6.

With tool-length offsets active, the Z-axis position display reads 0.00 when the active tool moves to Part Zero. Tool-length offsets simplify programming. To move to a position 0.5 inch into the work, program a move to a Z-.5 position.

Tool # 0 Z0.0

PartZero

Figure 1-6, Tool-Length Offset

CNC Programming and Operations Manual

P/N 70000504I - CNC Programming Concepts

Tool Diameter Compensation

When tool compensation is not active, the CNC positions the tools center on the programmed path. This creates a problem when programming a part profile because the cutting edge is half a diameter away from the path. Use tool diameter compensation to overcome this problem.

NOTE: Be familiar with basic CNC principles before attempting to write

When tool compensation is active, the CNC offsets the tool by half a diameter to position the cutting edge of the tool on the programmed path.

This allows you to program the coordinates along the part profile without adjusting the path to compensate for tool diameter.

Most moves can be compensated. Specify right or left compensation. Right or left refers to the side of the path to which the tool offsets, viewed from behind the tool as it moves.

NOTE: Tool compensation should be used only with lines and arcs.

compensated moves.

With left-hand tool compensation active, the tool offsets to the left of the programmed path (looking from behind the tool as it moves). Refer to

Figure 1-7.

LHCOMP

Figure 1-7, Left-Hand Tool Compensation

CNC Programming and Operations Manual

P/N 70000504I - CNC Programming Concepts

With right-hand tool compensation active, the tool offsets to the right of the programmed path (looking from behind the tool as it moves). Refer to

Figure 1-8.

RHCOMP

Figure 1-8, Right-Hand Tool Compensation

When the CNC encounters two consecutive, compensated moves, the tool follows the offset path for the first move until it reaches the offset path for the second move. Refer to

Figure 1-9. The tool may intersect the

offset path for the second move, either before or after the endpoint of the first move, depending on the geometry.

Move 2

Tool Path

Move 1 End Point

Move 1

Figure 1-9, Consecutive Compensated Moves

COMP2

The moves to and from compensated moves are called ramp moves. Ramp moves give the CNC time to position the tool. The ramp move must be at least half the active tool’s diameter in length.

CNC Programming and Operations Manual

P/N 70000504I - CNC Programming Concepts

At the start of a ramp move, the tool centers on the programmed path. At the end of the ramp move (starting point of the compensated move), the tool centers perpendicular to the starting point, offset by half the tool’s diameter. Refer to

Figure 1-10.

Figure 1-10, Ramping into a Compensated Move

Carefully consider how compensation will affect the position of the tool at the start and end of a move.

CNC Programming and Operations Manual

P/N 70000504I - CNC Programming Concepts

When a compensated move starts and stops in a corner, the tool gouges the work because the tool offsets to a position perpendicular to the endpoint. Begin ramp moves at the side to avoid gouging the workpiece. Refer to

Figure 1-11.

NOTE: Use canned cycles to cut profiles and pockets, when possible.

The CNC automatically selects ramp On/Off positions in a canned cycle.

Figure 1-11, Ramp On/Off Choices for Milling Inside a Square

CNC Programming and Operations Manual

Adj

pPar

P/N 70000504I - CNC Programming Concepts

Using Tool Diameter Compensation and Length Offsets with Ball-End Mills

When using a ball-end mill to cut contoured surfaces, use tool diameter compensation and tool-length offset together, if at all. Unlike an end cutter, the tool-length offset for a ball-end mill is not set to the tip of the tool.

Set the tool-length offset for a ball-end mill half the tool’s diameter back from the tip. Refer to length offsets, refer to “Section 10 - Tool Management.”

Figure 1-12. For more details on how to set tool-

Angle Measurement

Measure angles from the 3 o’clock position (0 degrees). Positive angles rotate in a counterclockwise direction; negative angles rotate in a clockwise direction. Refer to

Ball End Mill

QuillAtTool#0,Z0Position

Tool DiameterFrom Ti

Tool Length Offset

ustedToBall'sCente

tZero

Figure 1-12, Setting Tool-Length Offset for Ball End Mill

Figure 1-13.

Clock Reference

X-

Y+

Y-

Positive Angle

+30

Negative Angle

X+

Figure 1-13, Absolute Angle Measurement

CNC Programming and Operations Manual

P/N 70000504I - CNC Programming Concepts

Corner Rounding

Corner rounding permits the operator to blend the intersection of consecutive moves.

To activate corner rounding, the operator keys a radius value (positive) into the blends the endpoint of the first move with the starting point of the second. The blend starts where the radius is tangent to the first move, and extends to where the radius is tangent to the second.

Use corner rounding between two lines or two arcs. Also use corner rounding between non-tangent line and arc moves.

Line-to-Line Corner Rounding

When the first move contains a CornerRad value, the CNC automatically finds the radius center and the tangent points necessary to calculate the tool path. The resulting tool path follows the solid line. Refer to

CornerRad field of the first move. When the program runs, it

Figure 1-14.

Figure 1-14, Line-to-Line Corner Rounding

CNC Programming and Operations Manual

P/N 70000504I - CNC Programming Concepts

Line-to-Arc Corner Rounding

Figure 1-15.

NOTE: If the line move is already tangent to the arc move, the CNC

ignores corner rounding.

Figure 1-15, Line-to-Arc Corner Rounding

Arc-to-Arc Corner Rounding

When a CornerRad value is programmed into the first move, the CNC automatically finds the radius center and the tangent points necessary to calculate the tool path. The resulting tool path follows the solid line. Refer to

Figure 1-16.

Figure 1-16, Arc-to-Arc Corner Rounding

CNC Programming and Operations Manual

P/N 70000504I - CNC Programming Concepts

Chamfering

Chamfer between two consecutive line moves. A chamfer starts at a specified distance before the endpoint of the first move and ends the same distance from the starting point of the second move. To program a chamfer move, enter a negative value into the move. The entered value is the chamfer distance. The resulting tool path follows the solid line. Refer to

Figure 1-17.

CornerRad field of the first

Figure 1-17, Chamfering

CNC Programming and Operations Manual

P/N 70000504I - CNC Programming Concepts

Plane Selection

Circular moves and tool diameter compensation are confined to the plane you select (XY, XZ, or YZ).

CAUTION: A plane viewed from the wrong side causes arc

directions, angle references, and axis signs to appear

Refer to Figure 1-18 for a description of the three available planes.

reversed.

Figure 1-18, Plane Identification

CNC Programming and Operations Manual

P/N 70000504I - CNC Programming Concepts

Arc Direction

The standard rule is to view arc direction for a plane from the positive toward the negative direction along the unused axis. From this viewpoint clockwise (Cw) and counterclockwise (Ccw) arc directions can be determined. For example, in the XY plane, you view along the Z-axis, from Z+ toward Z-, to determine Cw/Ccw directions. The Cw/Ccw arc directions for each plane are shown in

Figure 1-19.

Figure 1-19, Clockwise and Counterclockwise Arc Directions

CNC Programming and Operations Manual

P/N 70000504I - CNC Console And Software Basics

Section 2 - CNC Console and Software Basics

Console

The CNC console consists of a 12.1” color, flat-panel Liquid Crystal Display (LCD), a keypad to the right of the monitor, and soft keys below the monitor. Refer to Figure 2-1.

LCD

Keypad

Soft Keys

Keypad

3000M CONSOLE

Figure 2-1, CNC Console

Refer to Figure 2-2. The keypad to the right of the monitor has four types of keys:

 Programming Hot Keys  Editing Keys  Manual Operation Keys  Operator Keys

Programming Hot Keys

Editing Keys

Manual Operation Keys Operator Keys

(with SPINDLE OVERRIDE)

3000M KEYPAD

Figure 2-2, Keypad

CNC Programming and Operations Manual

P/N 70000504I - CNC Console And Software Basics

Programming Hot Keys

Programming hot keys allow you to enter position coordinates and provide quick access to functions that speed up programming. They are active in the Edit and Manual Mode. Refer to Table 2-1.

Table 2-1, Programming - Hot keys

Label or Name Key Face Purpose X

Selects X-axis for position inputs.

ABS/INC

1/RAPID

2/LINE

3/ARC

4/FEED

5/TOOL

RAPID

LINE

FEED

TOOL

Selects Y-axis for position inputs.

Selects Z-axis for position inputs.

Selects U-axis for position inputs.

Switches CNC between Absolute and Incremental Modes.

Zero / Switches comment asterisk in edit mode. Switches resolution displa between program and Dist. To Go.

One / Hot key for programming a Rapid move.

Two / Hot key for programming a Line move.

Three / Hot key for programming an Arc.

Four / Hot key for changing feedrate. Five / Hot key for programming a

tool.

6/MCODE

7/UNIT

UNIT

Six / Hot key for programming an Mcode.

Seven / Hot key for switching between inches (Inch) and millimeters (mm).

8/DWELL

9/PLANE

+/-

DECIMAL/RPM

PLANE

Eight / Hot key for programming a Dwell.

Nine / Hot key for selecting a plane. Sign change / Toggle hot key.

Decimal point / Hot key for programming the spindle RPM.

(Continued…)

CNC Programming and Operations Manual

P/N 70000504I - CNC Console And Software Basics

Table 2-1, Programming - Hot keys (Continued)

Label or Name Key Face Purpose

CALC

Editing Keys

Editing keys allow you to edit program blocks. These keys are located below the Programming Hot Keys. Refer to Table 2-2.

Table 2-2, Editing Keys

Label or Name Key Face Purpose

CLEAR

ARROW

ENTER

Manual Operation Keys

Manual Operation Keys allow you to control machine movements manually. These keys are located below the Editing Keys. Refer to Table 2-3.

Calculators / Hot key to display the Select Type of Calculator: pop-up menu. See Figure 12-1, Calculator

Selection Menu.

C L E A R

Clears the selected messages, values, commands, and program blocks.

Allows you to move highlight bars and cursor around the screen.

Selects blocks for editing, activates menu selections, activates number entry, or presets XYZ positions.

Table 2-3, Manual Operation Keys

Label or Name Key Face Purpose JOG

Cycles the CNC through manual movement modes (JOG: RAPID,

JOG: FEED, JOG: 100, JOG: 10, JOG: 1).

U+

Manually moves machine in positive U direction.

U-

Manually moves machine in negative U direction.

Z+ Z- Y+ Y-

Manually moves machine in positive Z direction.

Manually moves machine in negative Z direction.

Manually moves machine in positive Y direction.

Manually moves machine in negative Y direction.

(Continued…)

CNC Programming and Operations Manual

P/N 70000504I - CNC Console And Software Basics

Table 2-3, Manual Operation Keys (Continued)

Operator Keys

Table 2-4, Operator Keys

Label or Name X+

X-

SERVO RESET

Key Face Purpose

Manually moves machine in positive X direction.

Manually moves machine in negative X direction.

Activates servo motors.

SPINDLE FORWARD

Starts spindle in a clockwise direction (viewed from the top of the motor). Optional.

SPINDLE REVERSE

Starts spindle in a counterclockwise direction (viewed from the top of the motor). Optional.

SPINDLE OFF

Stops the spindle.

Operator Keys allow you to control machine movements manually. These keys are located below the Manual Operation Keys and on the right side panel of the CNC console. Refer to Table 2-4.

Label or Name Key Face Purpose

FEEDRATE OVERRIDE

Overrides the feed and/or rapid rate of the axes in Manual, Auto, and Single Step modes. It is a 13-position rotary switch, which ranges from 0 to 120 percent. (Each increment adjusts the feedback override by 10%.)

NOTE: The override range for rapid rate is 100%. The CNC will not exceed the maximum rapid rate.

SPINDLE OVERRIDE

SPINDLE

Typically on the right side panel of the CNC console. Overrides the programmed spindle RPM rate. It is a 13-position rotary switch that ranges from 40 to 160 percent. (Each increment adjusts the spindle override by 10%.) This feature can be used only on machines with programmable spindles.

E-STOP

The red emergency stop button disconnects the machine’s servos, stopping the spindle and all machine movement.

(Continued…)

CNC Programming and Operations Manual

P/N 70000504I - CNC Console And Software Basics

Table 2-4, Operator Keys (Continued)

Label or Name Key Face Purpose

START

HOLD

The green moves except jog.

The red program or programmed move. (Press

START to resume.)

START key initiates all machine

HOLD key pauses any running

Soft Keys (F1) to (F10)

The soft keys (function keys) located just below the monitor are labeled (F1) through (F10). Soft key functions are not hard-wired but change in various modes. Active soft keys are labeled on screen. Inactive soft keys remain blank.

Off-line Keyboard (Optional)

The CNC supports most standard PC keyboards. Refer to “Section 13 Off-line Software.” All keypad inputs except are available on a keyboard.

E-STOP and SERVO RESET

Software Basics

Pop-up Menus

The CNC’s screens change as different modes are activated. Basic procedures and features of the software remain the same, regardless of the CNC’s mode.

Pop-up menus are temporary menus that allow you to make additional selections. Refer to Figure 2-3. Each pop-up menu contains a highlight bar. The

ENTER to activate the highlighted selection. Press the soft key that

activated it or press

ARROWS move the highlight bar up and down the menu. Press

CLEAR to close a pop-up menu.

POPUP3X

Figure 2-3, Pop-up Menu

CNC Programming and Operations Manual

P/N 70000504I - CNC Console And Software Basics

Screen Saver

After a set period of inactivity, the CNC’s screen dims to preserve the LCD. Press any key to restore the CNC to a ready status.

Switching Selections with the Toggle Key

Press the +/- key (toggle key) to toggle between options. (For example: Cw/Ccw, ToolComp.) This key also produces the negative symbol.

Clear Key

Press a message on the message line.

Operator Prompts

The CNC prompts when it requires specific information. When the CNC prompts for a text entry, use the ASCII Chart to enter ASCII characters from the keypad. Refer to “ASCII Chart” for more information. Enter numbers from the keypad.

ASCII Chart

When the CNC prompts for a text entry, the ASCII (F2) soft key is displayed. Press ASCII (F2) to toggle the ASCII Chart On and Off. The ASCII Chart allows you to enter text from the keypad. Refer to

Figure 2-4.

CLEAR to clear an entry in an entry field, a line from a program, or

ASCII

Figure 2-4, ASCII Chart Pop-up

Using the

ENTER key to display the character in the prompt area. Turn off the

ASCII Chart, and press

ARROW keys, select the character you want to enter. Press the

ENTER to complete the text entry.

CNC Programming and Operations Manual

P/N 70000504I - CNC Console And Software Basics

Cursor and Highlight Functions

The CNC uses either a cursor or highlight to mark an item for selection or editing.

The highlight is displayed in the Edit Mode, Program Directory, Manual mode, and ASCII Chart. Use the

ARROWS to move the highlight. The

software highlights a selected item in a menu or window. Selected items can be activated or changed in some way. For instance, you highlight a program block in Edit Mode to edit it. You highlight an entry field label in a Graphic Menu to enter a value or switch between the available choices.

The cursor is displayed when the Tool Page activates. The cursor is a white underline that indicates where letters and numbers will be inserted.

Entering Text

Use the ASCII Chart or a keyboard to enter text. To enter text using the ASCII (F2) chart:

1. Press ASCII (F2). ASCII Chart activates.

2. Highlight desired character.

3. Press

ENTER. The CNC displays the selected character at the

cursor.

4. Select all required characters.

5. Press ASCII (F2) to close the ASCII Chart.

Typing Over and Inserting Letters and Numbers

The ASCII Chart has two text entry modes: Typeover (default) and Insert.

In the Typeover Mode, new characters replace characters marked by the cursor.

In the Insert Mode, new characters appear at the cursor and existing characters move to the right. When the Insert Mode is active, Ins (F3) highlights.

To put the CNC in the Insert Mode:

1. When the CNC prompts for a name, press Ins (F3). Ins (F3) highlights.

CNC Programming and Operations Manual

P/N 70000504I - CNC Console And Software Basics

Deleting Characters

To delete characters:

1. With the ASCII Chart active, move the cursor to underline the character being deleted.

2. Press Del (F4). The selected character disappears.

NOTE: Press

Messages/Error Messages

Messages generated by the CNC appear in the message area, present in all program-running modes. Refer to Figure 2-5. When the CNC generates more than one message, the message with the highest priority is displayed in the message area. Lower-priority messages remain in memory. The on-screen MESSAGE label highlights when pending messages remain in memory. There are two ways to review pending messages:

 Press CLEAR. The CNC clears the current message and displays the

next message.

 From the Manual screen, press MESSAGE (F1). Displayed

messages appear in the Program Area of the screen.

Some messages are advisory; others stop CNC operation. For those that stop operation, you must put the CNC in the Manual Mode to correct the problem, and then clear the message.

CLEAR to delete an entire word.

% :

100

Figure 2-5, Messages Display

CNC Programming and Operations Manual

P/N 70000504I - Manual Operation and Machine Setup

Section 3 - Manual Operation and Machine Setup

Powering On the CNC

To power on the CNC:

1. Press the power switch on the CNC cabinet. The CNC activates the startup screen and prompts you to Press F10 to continue.

2. Press C

3. Highlight CNC Control, and press

Shutting Down the CNC

To shut down the CNC:

1. Press

2. Press EXIT (F10) to display the Software Options menu.

3. Press the power switch on the CNC cabinet to power down the CNC.

Emergency Stop (E-STOP)

Use E-STOP to take all axes and spindle servos offline and halt machine movement.

To reset

1. Rotate the E-STOP switch in the direction of the arrows. The switch clicks when reset. The CNC does not automatically reactivate the servos after an machine or start the spindle.

2. Press

ONT. (F10) to display the Software Options menu.

ENTER to activate Manual Mode.

E-STOP to disengage the Servos and activate Manual Mode.

E-STOP:

E-STOP reset. You must reset the servos to move the

SERVO RESET to reset the servos.

Performing an Emergency Stop

To perform an emergency stop:

1. Press

NOTE: You cannot activate E-STOP using an off-line keyboard.

E-STOP to disengage the servos and activate Manual Mode.

CNC Programming and Operations Manual

P/N 70000504I - Manual Operation and Machine Setup

Activating/Resetting the Servos

For safety reasons, the CNC powers up with the servo motors off. With the servos turned off, the CNC cannot move the machine and the spindle will not start. The CNC displays the SERVO OFF! message when the servos are off. Refer to “Section 2 - CNC Console and Software Basics” for reviewing messages.

During operation, press automatically turn off if the machine attempts to power past a limit switch.

To reset the servos:

1. After a limit switch has been tripped, the servos turn off. Manually reposition the machine inside its range of travel.

2. Press

3. Rotate the switch in the direction of the arrows to reset switch clicks when reset.

4. Press

NOTE: You cannot activate the servos using an off-line keyboard.

(Re-)Starting the Spindle

SPINDLE FORWARD and SPINDLE REVERSE do not work if E-STOP is active or

if the servos go off-line. To (re-)start the spindle:

1. Reset

2. Press

E-STOP to turn off the servos. Servos

E-STOP.

E-STOP. The

SERVO RESET to reset the Servos.

E-STOP. SERVO RESET.

3. Press either

SPINDLE FORWARD or SPINDLE REVERSE, as required.

CNC Programming and Operations Manual

P/N 70000504I - Manual Operation and Machine Setup

Manual Mode Screen

The Manual Mode screen is the main CNC screen. All other operating screens activate from the Manual Mode screen. In Manual Mode, the

MANUAL (F4) soft key label highlights. Refer to Figure 3-1.

Figure 3-1, Manual Mode Screen

The Manual Mode screen features:

Position Display Machine Position Display

Displays X, Y, and Z position coordinates. Displays the axis positions in reference to

Machine Home. (Not shown when Draw activates.)

Secondary Display Area Primary Display Area

Displays essential operating information. Displays additional operating information.

(Not shown when Draw activates.)

Message Area

Displays messages, prompts, and reminders.

Soft Key Labels

Identify the function of the soft key directly underneath. Labels change from screen to screen. A highlighted label indicates an active mode.

Program Listing

Displays program blocks as they run in Auto or S.Step Mode.

Soft Key Labels

CNC Programming and Operations Manual

P/N 70000504I - Manual Operation and Machine Setup

Primary Display Area Labels

BLOCK: TOOL: FEED: POSN:

DIA: %:

Secondary Display Area Labels

PROGRAM MANUAL/AUTO/S.STEP IN-POSN

ABS/INC INCH/MM HALTED/*HALTED/

RUNNING

Current program block number. Active tool. Current feedrate. Position Display Mode (Program or

Distance to Go). Active tool diameter. Feedrate override setting (0% to 120% for

Feed moves, 0% to 100% for Rapid moves).

Name of selected program. Current operating mode. Indicates whether the machine has

reached target (in-posn) or not. Current positioning mode. Current units mode.

HALTED (without asterisk) indicates

machine is in a programmed hold, or has completed its program.

*HALTED (with

asterisk) indicates hold was activated by an event, or

HOLD was pressed. RUNNING

indicates normal program run.

FEED/RAPID/ARC: LOOP:

Current move mode. Number of loops remaining (when running

a subprogram that has loops).

DWELL: FIXTURE: RPM:

Seconds remaining in a dwell. Active fixture offset number. Spindle RPM (Optional). May display

programmed RPM or actual RPM. Refer to builder’s documentation for details.

Spindle override setting (40% to 160%) Optional.

JOG:

Current jog mode.

SPINDLE: Spindle status (FWD/REV/OFF).

Optional.

COOLANT:

Coolant status. Optional.

CNC Programming and Operations Manual

P/N 70000504I - Manual Operation and Machine Setup

PARTS:

Counts the number of successfully completed parts. (Increments by 1 every time the CNC encounters EndMain in a program run.) The counter resets to zero when you start a new program. (Refer to “Section 8 - Running Programs.”)

Position Display

TIMER: Total program run time from

START to

EndMain execution. If the CNC holds,

the counter pauses until the program restarts. The counter resets to 0 (zero) when you start a new program. (Refer to “Section 8 - Running Programs.”)

Refer to Figure 3-2. The POSN: option sets the CNC to display machine position in one of two ways:

Program

Position Display shows the programmed position.

Distance To Go

Position Display shows the remaining distance to the commanded position. (DISTTOGO)

To switch the P

OSN: setting:

1. In Manual, S. Step, or Auto Mode, press 0 (zero) to switch the setting between PROGRAM and DISTTOGO.

Soft Key Labels

Figure 3-2, Position Display Options

CNC Programming and Operations Manual

P/N 70000504I - Manual Operation and Machine Setup

Manual Machine Operation

Two types of manual operation are available:

 Manual Mode Digital Readout. Use handles to move the

machine. Servos deactivate.

 Auto Mode Control machine using the keypad. Servos move

the machine.

Manual Mode

In DRO Mode, the CNC acts as a digital readout and you use handles to move the machine.

To activate Manual Mode:

Auto Mode

1. Press

E-STOP.

2. Locate the MANUAL/AUTO switch, usually located on the back of the console.

3. Set the switch to MANUAL. Servos and spindles disconnect.

4. Reset

5. Press

E-STOP. SERVO RESET to reactivate the spindle.

To activate Auto Mode:

1. Press

E-STOP.

2. Locate the MANUAL/AUTO switch and move the switch to AUTO.

3. Reset

4. Press

E-STOP. SERVO RESET. The servos reactivate and the CNC now

operates the machine.

CNC Programming and Operations Manual

P/N 70000504I - Manual Operation and Machine Setup

Mode Settings

The operator controls every aspect of the CNC’s operation. Settings that remain active for more than one operation or event are said to be modal. These settings remain active until changed or turned off.

Many of the CNC’s features are modal. For example, move type (Rapid or Feed), feedrate (IPM), units (Inch or MM) or ABS/INCR.

The operator should make all of the mode adjustments required for the machine to move properly before making a manual move. Modes set from the Manual screen remain active until changed.

Refer to Table 3-1 for the modes/settings from the Manual screen.

Table 3-1, Manual Mode Settings

Mode/Setting Name Choices

Position Mode

Units Mode Move Mode Plane Active Tool

Absolute/Incremental Inch/Millimeter Rapid/Feedrate XY/YZ/XZ Tool Diameter Compensation and

Tool-Length Offsets

The operator can use the Manual screen to program the locations of the Absolute Zero Reference (X0, Y0) and the tool change position (Z0, Tool #0).

The following four types of moves are available in Manual Mode:

 Jog (Conventional)  Jog (Continuous)  One Shot Move  Manual Data Input (MDI)

CNC Programming and Operations Manual

P/N 70000504I - Manual Operation and Machine Setup

Activating Manual Mode Rapid or Feed

Press JOG to switch the Jog Mode. Two Jog Modes (Rapid and Feed) are CNC move modes. The CNC displays the active Rapid/Feed Mode in the Secondary Display Area.

Setting a Feedrate

You can change the feedrate at any time. When

FEEDRATE OVERRIDE is

set to 100%, the CNC executes Feed moves at the specified feedrate. Adjust the active feedrate with

FEEDRATE OVERRIDE adjusts the feedrate by an increment of ten. FEEDRATE OVERRIDE has a range of 0% to 120%. Align the knob pointer

FEEDRATE OVERRIDE. Each click of

with the white stripe to set the override to 100% (no override). To change the active feedrate:

1. In Manual Mode, press the 4/

FEED hot key. The CNC prompts for a

value.

2. Enter the desired feedrate and press Save (F10) or

ENTER to return to

the Manual screen.

3. Press

START to activate the feedrate change.

– or –

Press Manual (F4) to cancel the feedrate change.

CAUTION: If the CNC is shut down, then powered up again, the

manufacturer’s setup file will reload the CNC’s default feedrate.

Adjusting Rapid Move Speed

Use

FEEDRATE OVERRIDE to adjust the Rapid move speed. Every click of

FEEDRATE OVERRIDE adjusts the Rapid move speed by 10% of the default

speed, with a range of 0% to 100%. Align the knob pointer with the white stripe on the console to set the override to 100% (no override).

CNC Programming and Operations Manual

P/N 70000504I - Manual Operation and Machine Setup

Overriding the Programmed Spindle RPM

You can change the programmed spindle RPM at any time. Adjust the programmed RPM with

Table 2-4, Operator Keys. Each click of the spindle speed by 10%. The 160%. Align the knob pointer with the white stripe to set the override to 100% (no override).

Absolute/Incremental Modes

The CNC recognizes both absolute and incremental positions and can switch between the two modes at any time. In the Absolute Mode, the CNC measures all points from Absolute Zero. In the Incremental Mode, the CNC measures the next move from its present position. The active position mode is displayed in the Secondary Display Area.

 ABS indicates Absolute Mode  INC indicates Incremental Mode

To activate the Absolute or Incremental Mode:

1. Put the CNC in the Manual Mode.

2. Press

ABS/INC to toggle the setting.

Inch/MM Modes

SPINDLE OVERRIDE. Refer to

SPINDLE OVERRIDE adjusts

SPINDLE OVERRIDE range is 40% to

The CNC uses two units of measurement, Inch and Millimeter. In Inch Mode, the CNC counts in inches. In Millimeter Mode, the CNC counts in millimeters.

Change the unit’s mode from the Manual screen or in a program. The CNC displays the active units mode in the Secondary Display Area. To activate the Inch or Millimeter Mode:

1. With the Manual screen active, press 7/

UNIT to change the active

Units Mode (Inch/mm). The Secondary Status Area displays the current mode.

CNC Programming and Operations Manual

P/N 70000504I - Manual Operation and Machine Setup

Setting Absolute Zero

Absolute Zero is the point the CNC recognizes as X0, Y0 in the Absolute Mode. The CNC measures all absolute XY positions from this point.

The CNC uses a floating Absolute Zero. You can locate Absolute Zero anywhere within or beyond the machine’s range of travel.

At power-up, the current machine location becomes Absolute Zero (X0, Y0, and Z0). At power down, Absolute Zero is lost. Setting Absolute Zero to a location on the part is called setting Part Zero.

NOTE: For machines without homing, it may be necessary to set

NOTE: The active tool-length offset determines the Z-Axis Part Zero

(Z0).

NOTE: Use a Home function to define a permanent Absolute Zero

(Machine Home).

Defining Absolute Zero in X and Y Axes

To define Absolute Zero in X and Y:

1. Position the center of the spindle at the required part zero position.

2. In Manual Mode, press X. The CNC prompts for X Axis Part Zero position and displays 0.00.

3. Press Y. The CNC prompts for Y Axis Part Zero position and displays 0.00.

4. Press

ENTER to accept the entered values (X0, Y0).

Presetting the X- or Y-Axis

To preset the X- or Y-axis to a predetermined position:

1. Adjust the machine’s position to a known distance from the desired Part Zero.

2. Press X. The CNC prompts for the X Axis Part Zero position and displays 0.00.

3. Enter the desired X Axis position (include sign) and press Y. The CNC prompts for the Y Axis Part Zero position and displays 0.00.

4. Enter the desired Y Axis position (include sign), and press set the new position coordinates.

ENTER to

CAUTION: To enter positions, press ENTER and not START. START

will initiate a move to the entered coordinates.

CNC Programming and Operations Manual

P/N 70000504I - Manual Operation and Machine Setup

Fixture Offsets (Work Coordinate System)

Sometimes it is convenient to be able to shift Part Zero with more than one coordinate system. (For example, if you must machine two or more workpieces in the same setup.) When you use multiple coordinate systems, you assign a different Part Zero for each workpiece. This simplifies programming because you can enter the moves required to machine a part from any selected reference point.

All Absolute moves are referenced from the active Fixture Offset location. The Fixture Offset location is referenced from Machine Home. You can define up to nine Fixture Offsets in the Fixture Offset Table. Refer to

Figure 3-3.

Figure 3-3, Locating Fixture Offsets

When you choose the location of Fixture Offsets, consider the following:

• Choose a reference point that corresponds to the information provided

on the part print.

• Be consistent. To prevent confusion, use the same offset location for

each part. (In the diagram, this is the upper-left corner.)

• The distance between the Fixture Offset and Machine Zero on each

axis is the value entered in the Fixture Offset Table. Include the ± direction of movement. For the diagram above:

Fixture Offset # Coordinates Entered in Fixture Offset Table

FixOff #1 X-9.124, Y-7.655, Z (not shown) FixOff #2 X-4.862, Y-3.862 Z (not shown) FixOff #3 X-2.431, Y -2.440 Z (not shown)

CNC Programming and Operations Manual

P/N 70000504I - Manual Operation and Machine Setup

Fixture Offset locations also can be used to preset the current location to entered coordinates or reset the current machine position to 0, for selected axes. (Refer to “Section 4 - Writing Programs” for information on how to program Fixture Offsets and use the Fixture Offset Table.)

Setting Tool Change Position

The tool change position is usually the fully retracted position of the quill, set to Tool #0, Z0 (no tool-length offsets, Part Zero). The Tool #0, Z0 position is often used for tool changes or as a safe place to make rapid XY moves.

At power up, the current location is Tool #0, Z0. This position is not stored in memory when you shut down the machine.

Set Tool #0, Z0 before setting tool-length offsets. Changing the location of Tool #0, Z0 alters all tool-length-offset settings.

Refer to “Section 1 - CNC Programming Concepts” and “Section 10 - Tool Management” for more information on tool-length offsets.

NOTE: For machines without homing, it may be necessary to set

NOTE: Program a move to Z0 with XY rapid moves. This will ensure

that the quill clears the surface of the work during the rapid move, thus avoiding possible tool or machine damage.

Locating Tool #0, Z0

NOTE: This procedure is necessary only if your machine does not have

homing capability.

To locate Tool #0, Z0:

1. In Manual Mode, press the

5/TOOL hot key to display the TOOL

MOUNT Help Graphic.

2. Press Save (F10). The CNC prompts you to Press

MANUAL to Cancel.

START or execute

3. Press

START to activate tool #0 and deactivate length offset.

4. Adjust the machine to the desired tool change or tool #0, Z0 position.

5. Press Z. The CNC prompts for absolute Z-Axis position and displays

0.00.

6. Press

ENTER. The CNC displays 0.00 on Z.

CNC Programming and Operations Manual

P/N 70000504I - Manual Operation and Machine Setup

Presetting the Z-Axis

To preset the Z-axis to a predetermined position:

1. In Manual Mode, go to Tool #0, Z0.

2. Press Z. The CNC prompts for the absolute Z Axis position and displays 0.00.

3. Enter the Z-Axis position (including sign), and press

Activating a Tool

Activate a tool to allow applicable length offset and diameter listed in the Tool Page. Refer to “Section 4 - Writing Programs” to activate a tool in a program.

To manually activate a tool:

1. In Manual Mode, press

2. Enter a tool number, and press Save (F10) to return to Manual Mode.

3. Press

Press

Activating a Plane

Default plane: XY.

ENTER. The Z

Axis display changes to the entered position. This indicates that the CNC has preset Z to the entered position.

5/TOOL. The CNC prompts for the tool

number.

START. The CNC displays the active tool number in the Primary

Display Area.

– or –

MANUAL (F4) to cancel the selection.

To change the active plane:

1. In Manual Mode, press

9/PLANE. The CNC prompts for a plane

selection.

2. Press the +/- key to switch to the desired plane selection.

3. Press Save (F10) to return to Manual Mode.

4. Press

START to activate the selected plane.

– or –

Press

MANUAL (F4) to cancel the selection.

CNC Programming and Operations Manual

P/N 70000504I - Manual Operation and Machine Setup

Activating a Spindle RPM (Requires Programmable Spindle Option)

To activate a spindle RPM:

Jog Moves

1. In Manual Mode, press the

(Decimal/RPM) key. The CNC prompts

for a RPM value.

2. Enter the desired RPM value, and press Save (F10) to return to Manual Mode.

3. Press

START to activate the selected spindle RPM.

– or –

Press

MANUAL (F4) to cancel the selection.

Use the Manual Operation Keys to make jog moves. There are two keys for each axis of motion, one for the positive direction and one for the negative direction. Refer to Figure 3-4.

Enable Jog moves when:

• The CNC is in the Manual Mode, Teach Mode, or Tool Page.

• The servos are on.

Figure 3-4, Manual Operation Keys

CNC Programming and Operations Manual

P/N 70000504I - Manual Operation and Machine Setup

There are five available move modes. The machine builder determines the rate for each mode (Jog Rapid and Jog Feed) at machine setup. Press

JOG to cycle through the available Jog settings. Refer to Table 3-2.

Table 3-2, Move Mode Selections

Mode Description Rapid

Default rapid speed for continuous jogs. Actual speed determined at machine setup.

Feed Jog: 100

Continuous jog at current feedrate. Conventional Jog Mode, increment set to 100 times

resolution of machine.

Jog: 10

Conventional Jog Mode, increment set to 10 times resolution of machine.

Jog: 1

Conventional Jog Mode, increment set to actual resolution of machine.

In Manual Mode, the operator can change the Jog Mode anytime.

Changing the Jog Mode

To change the Jog Mode:

1. In Manual Mode, press

JOG to change the mode selection. The CNC

displays the selected mode in the Secondary Display Area.

2. Press

JOG repeatedly to cycle through the available Jog settings.

NOTE: You can change the Jog Mode from the Manual Mode, Teach

Mode, or Tool Page.

Jogging the Machine (Conventional)

To jog the machine one increment at a time:

1. In the Manual Mode, Teach Mode, or Tool Page, press through the available settings:

JOG: 100, JOG: 10, or JOG: 1. The CNC

JOG to cycle

displays the selected setting in the Secondary Display Area.

2. Press the required axis key (

X+, X-, Y+, Y-, Z+, or Z). Every time you

press an axis key, the machine jogs along the selected axis at the indicated increment (100, 10, or 1 times machine resolution).

CNC Programming and Operations Manual

P/N 70000504I - Manual Operation and Machine Setup

Jogging the Machine (Continuous)

To jog the machine along an axis continuously:

1. In Manual Mode, Teach Mode, or Tool Page, press through the available settings. Set the machine to

FEED. The CNC displays the selected setting in the Secondary Display

Area.

2. Press the required axis key ( Rapid or Feed Mode along the selected axis until you release the key.

Operating the Handwheel (Optional)

The system supports an option that allows you to jog a selected axis using a remote handwheel.

NOTE: The handwheel operation described here assumes that the

optional handwheel has been properly installed and configured.

The resolution of the handwheel depends on the selected Jog Mode. The CNC displays the selected Jog Mode on the screen.

Press the “Jog Moves” in this section for more information on selecting a Jog Mode. The handwheel works only in conventional Jog Modes (100, 10, and 1).

To operate the handwheel option:

1. From the Manual screen, press the key highlights and the other soft keys are blank. The Select HW Axis popup menu activates. Refer to Figure 3-5.

JOG key to cycle through the available Jog Modes. Refer to

JOG to cycle

JOG: RAPID or JOG:

X+, X-, Y+, Y-, Z+, or Z). The machine jogs in

HANDWHL (F8) soft key. The soft

Figure 3-5, Handwheel Axis Selection Pop-Up

NOTE: The handwheel soft key will not display unless the Setup Utility

has been configured for handwheel use.

2. From the Select HW Axis menu, highlight the axis that will be moved using the remote handwheel. Press

ENTER. You can now move the

selected axis using the remote handwheel.

CNC Programming and Operations Manual

P/N 70000504I - Manual Operation and Machine Setup

3. Press the JOG key to select a Jog Mode: 100, 10, or 1. The axis will move 100, 10, or 1 times the machine resolution, respectively, per click of the handwheel.

4. Move the handwheel clockwise to move the selected axis in a positive direction, or counterclockwise to move the axis in a negative direction.

One-Shot Moves

In Manual Mode, you can position the machine using one-shot moves. One-shot moves can be in Absolute or Incremental Mode in Rapid or Feedrate.

To execute a one-shot move:

Manual Data Input

1. In Manual Mode, press

JOG to select a move mode.

NOTE: All Jog modes, except Rapid Jog, run in Feed Mode.

2. Press ABS/INC to select a Positioning Mode (ABS/INC).

3. Enter the appropriate

4. Press

START.

X, Y, and Z coordinates.

NOTE: To pause one-shot moves, press HOLD. To resume, press

START. To cancel one-shot moves, press MANUAL (F4).

CAUTION: Press START, not ENTER, to initiate a one-shot move. If

you inadvertently press ENTER, Absolute Zero moves to the entered position.

NOTE: The 1/RAPID or 2/LINE hot keys also can initiate one-shot moves.

Activate the Absolute/Incremental Mode before you select the Rapid/Line Mode.

Manual Data Input (MDI) provides a quick way to program a single move, or a series of moves.

NOTE: From the Manual Data Input Mode, you can access all

programming options and write a complete part program.

The CNC stores MDI blocks in a permanent program named MDI.M. Write MDI blocks the same way as program blocks. The MDI editor has the same features as the regular Program editor. Press Draw to test MDI moves.

The MDI screen resembles the Edit screen with MDI.M listed as the active program. Refer to Figure 3-6. The moves in MDI remain in the MDI.M program until cleared or edited. Run the MDI.M program at any

CNC Programming and Operations Manual

P/N 70000504I - Manual Operation and Machine Setup

time. If you accidentally delete the MDI.M program, the CNC automatically creates a new one the next time the MDI Mode activates.

To save the MDI.M program, rename it. (Refer to “Section 9 - Program Management” for instructions.)

Figure 3-6, Manual Data Input (MDI) Screen

To execute an MDI command:

1. From the Manual screen, press MDI (F7) to display the Program Editor. The CNC automatically loads the MDI.M program and displays the program name on the bottom right part of the screen.

2. Enter the required program blocks.

3. If necessary, verify moves in Draw.

4. Press Exit (F10) to return to the Manual screen.

5. Press

START to execute the MDI move.

– or –

Press MANUAL (F4) to cancel the MDI move. NOTE: Refer to “Section 4 - Writing Programs” for instructions on how

to write program blocks.

CNC Programming and Operations Manual

P/N 70000504I - Manual Operation and Machine Setup

Disengaging the Z-Axis Drive System

The 3000M provides the capability to switch between two-axis and threeaxis operation. In Manual mode, just loosening the quick-release knob on the front of the Z-axis drive system can disengage the Z-axis. To reengage the Z-axis drive system, lift the quill handle until you feel the drive assembly becomes seated, then tighten the quick release knob.

In Automatic mode, program a ZMode TwoAxes or a ZMode ThreeAxes to specify the particular area of the program that should be ran in twoaxes or three-axes, respectively. When a ZMode TwoAxes is run in a program, the operator is prompted to disengage the Z-axis. When a ZMode ThreeAxes is run in a program, the operator is prompted to reengage the Z-axis. Once the Z-axis re-engaged, the operator can jog the Z-axis to the homing mark on the front of the Z-axis drive system and perform a Homing sequence. Refer to ZMode block in “Section 5, Drilling Cycles” for more details.

When a program or a section of a program is ran in two-axes mode, the operator is prompted to manually position the Z-axis as needed.

CNC Programming and Operations Manual

P/N 70000504I - Writing Programs

Section 4 - Writing Programs

Program Basics

Each program consists of blocks of instructions that direct machine movements. Give each program a unique name.

Many settings remain active until changed or turned off. These are modal settings. For example, move type (Rapid/Feed), feedrate (IPM), units (Inch/MM), or ABS/INCR.

Write programs with combinations of moves, mode changes, and canned cycles. The CNC has a built-in library of canned cycles stored in its permanent memory.

Developing Part Programs

First, decide how to clamp the part and where to set Part Zero (Absolute Zero). Locate Part Zero at a point on the work positively positioned by the clamping fixture. This allows consistent machining of subsequent parts. Since Absolute positions are measured from Part Zero, locate Part Zero at a convenient location.

Determine the required tools and set the length offset for each tool. If necessary, adjust the position of the knee so that the longest tool clears the top of the part in a Rapid, Tool #0 move to Z0. Treat tool information like part of the program.

Refer to the blueprint to select a Part Zero. Note the moves, positions, and tools needed to cut the part. The CNC has a calculator that finds coordinates for complex geometric shapes (refer to “Section 12 Calculators”).

To develop a part program:

1. Go to the Program Directory (the PROGRAM screen) and create the program for the part (refer to “Section 9 - Program Management”).

2. Go to the Program Editor (the Edit screen) to open the new program and begin to write blocks (refer to “Section 6 - Editing Programs”).

3. The first block in a program is usually an Absolute Mode block. Put the CNC in the Absolute Mode at the start of a program to enable absolute positioning. (Use Incremental Mode only when specifically needed.)

4. Put the CNC in the appropriate Inch/MM Mode in the second block.

5. In the first move of the program, rapid to Tool #0, Z0 to retract the quill fully for the next move.

6. In the second move, rapid to a convenient part-change position.

CNC Programming and Operations Manual

P/N 70000504I - Writing Programs

7. Execute moves toward a part in two steps: A Rapid X, Y move at a clear height, followed by a Z move to 0.1 inch (2mm) above the surface of the cut (standard starting height). If necessary, activate the first tool mount at this time.

NOTE: Program tool changes in separate blocks to make them easier to

find.

8. Subsequent blocks in the program are the moves, cycles, and tool changes required to machine the part.

9. Make the last three blocks of the program as follows: a) a Rapid move to Tool #0, Z0, b) a Rapid XY move to the same part change position used at the start of the program, and c) an EndMain block.

10. To verify and troubleshoot finished programs, run them in Draw Graphics Mode. Refer to “Section 7 - Viewing Programs with Draw.”

11. Secure the work on the table with the appropriate work-holding device.

12. Go to the Manual screen and set Part Zero at a convenient point on the part. Refer to “Section 3 - Manual Operation and Machine Setup.”

13. Go to the Tool Page and organize the tooling. Assign each tool a number (in the order of use). Assign length offset and tool diameter as appropriate. Refer to “Section 10 - Tool Management.”

14. If Fixture Offsets are used, define them in the Fixture Offsets Table. Refer to “Programming Fixture Offsets” in this section.

15. Before you cut a part, perform a dry run. There are several ways to get a close look at the programmed moves. Run the program in Motion Mode to hold between each move or in Single-Step Mode to hold between each block. Run the program with no tool installed, or with a tool installed, but the knee lowered so the tool never contacts the work.

16. After a successful dry run, the program is ready for production. Back up the program for safekeeping. Refer to “Section 9 - Program Management.”

CNC Programming and Operations Manual

P/N 70000504I - Writing Programs

Writing Program Blocks

You can program a block for a move type, mode, or cycle using one of the following: hot keys, soft keys, or pop-up menus.

To program a block, activate its graphic menu and fill in the appropriate values. To save a program block, press Save (F10) or press the last entry field in the graphic menu. The CNC adds the new block to the Program Listing.

The <End Of Program> block is the last line of a program. The CNC automatically numbers new blocks and inserts them in front of the

<End Of Program> block.

Using Graphic Menus

The Program Editor displays full screen graphic menus to write and edit program blocks. Refer to Figure 4-1.

ENTER on

Figure 4-1, Sample Graphic Menu

Graphic menus activate with the first entry field highlighted. To enter values, highlight the appropriate entry field, and press

ENTER to advance

the highlight to the next entry field. With the last entry field highlighted, press

ENTER to close the menu and add the block to the program.

Press Save (F10) from any entry field to close the graphic menu and add the block to the program. Move the highlight from field to field using the

ARROW keys. Fill out entry fields in any order.

CNC Programming and Operations Manual

P/N 70000504I - Writing Programs

Press CLEAR to remove values in the highlighted field. There are two types of entry fields in a graphic menu:

Optional entry fields Blank when the graphic menu activates. Required entry fields Contain 0.000 when the graphic menu

activates.

Required entry fields contain a 0.0000 default value. Change the value as required. Optional entry fields do not require a value. When left blank, the CNC usually assumes a default value or position. If the optional field is a position, the value defaults to the current position. If the optional field is a mode or tool change, the current mode and tool remain active. If the optional field is an angle, the value defaults to 0.0 degrees.

Type decimal points and negative signs where needed. Otherwise, the CNC assumes a positive whole number.

Press +/- to insert a negative sign or toggle selections in some entry fields (for example, Cw/Ccw fields).

No Move Blocks

Programming an Absolute/Incremental Mode Change

Programming an Inch/MM Mode Change

No Move Blocks does not initiate machine moves. Use No Move Blocks to set modes (Incremental/Absolute, etc.), activate tools (Tool#), and set feedrates (Feed).

A Dim (dimension) block sets the Absolute (Abs.) or Incremental (Incr.) Mode.

To program a Dim block:

1. In Edit Mode, press

ABS/INC. The SET ABS/INCR DIMENSION

graphic menu prompts you to select Abs or Incr.

2. Press +/- to toggle the mode.

3. Press Save (F10) or

ENTER to add the block to the Program Listing.

A Unit block sets the Inch (Inch) or Millimeter (MM) Mode. To program a Unit block:

1. In Edit Mode, press

7/UNIT. The SET INCH/MM UNIT graphic menu

prompts you to select Inch/MM.

2. Press +/- to toggle the selection.

3. Press Save (F10) or

ENTER to add block to the Program Listing.

CNC Programming and Operations Manual

P/N 70000504I - Writing Programs

Programming a Tool Change

Identify tools with tool numbers. When you activate a tool, its tool length and diameter offsets activate. List these values on the corresponding row of the Tool Page. Refer to “Section 10 - Tool Management” for information on the Tool Page.

NOTE: The CNC also activates listed coolant (optional) and spindle

operations (optional).

Tool-length offset remains in effect until a different tool activates. Always turn off tool-diameter compensation and ramp off before activating a new tool.

NOTE: You can program tool numbers with most moves; they do not

require a separate block. Each time a tool activates, the CNC holds the program to permit installation of the new tool. Programming unnecessary tool changes slows down production.

Activate Tool #0 to set the tool-length offset and diameter to 0.0. To change a tool:

NOTE: An absolute move to Tool #0, Z0 fully retracts the quill. An

incremental command to Z0 maintains the current position.

1. In Absolute Mode, program a Rapid Z0, Tool #0 to cancel length offsets and retract the quill to a safe position.

2. Program a Rapid move to the tool change XY position (usually Machine Zero).

3. Program a block to activate the required tool (example: Tool#1). When the CNC encounters the Tool# command, it holds optional spindle and coolant functions. The operator can now change the tool.

4. Press

START to resume operation. The CNC activates applicable tool

compensation, spindle, and coolant activities.

NOTE: Program tool changes in separate blocks to make them easier to

find.

Activating a Tool

To activate a tool:

1. In Edit Mode, press

5/TOOL. The TOOL MOUNT graphic menu

prompts for Tool #.

2. Type tool number and press

ENTER to add the Tool# block to the

Program Listing.

CNC Programming and Operations Manual

P/N 70000504I - Writing Programs

Activating Tool-Diameter Compensation

Refer to “Section 1 - CNC Programming Concepts” for basic information on tool-diameter compensation. You can compensate most move types. Compensation is modal and remains active until you cancel or change it.

Turn compensation on or off in (Rapid or Line) ramp moves. Ramp moves offset the tool on the programmed path by half the tool diameter. Tool compensation affects all subsequent moves until canceled.

The ToolComp command, available in Line or Rapid graphic menus, sets the required tool compensation. Settings include:

• Left (of the path)

• Right (of the path)

• Off (cancel compensation)

When the field is left blank, the current compensation, if any, remains in effect.

Many canned cycles include automatic tool compensation. Activate the correct tool diameter to ensure accuracy in these cycles. The required tool activates within the cycle.

Refer to Table 4-1 for a list of move and cycle compensation requirements.

Table 4-1, Move and Cycle Compensation Requirements

Move or Cycle Program a Rapid or Line

move to activate tool comp before you program the move or cycle. Tool diameter must be active.

Rapid Line Modal Arc Ellipse

X --X --X --X --X ---

(Has special requirements. Refer to “Section 5 - Programming Canned Cycles, Ellipses, and Spirals” for more information.)

Spiral

--- ---

(No compensation available.)

Activate/deactivate compensation automatically when you program the move or cycle. Tool diameter must be active.

(Continued…)

CNC Programming and Operations Manual

P/N 70000504I - Writing Programs

Table 4-1, Move and Cycle Compensation Requirements (Continued)

Move or Cycle Program a Rapid or Line

move to activate tool comp before you program the move or cycle. Tool diameter must be active.

Face

--- X

(Affects only step-over.)

Rectangular Profile

--- X

Cycle Circular Profile Cycle Rectangular Pocket

--- X

Cycle Circular Pocket Cycle Frame Pocket Cycle Irregular Pocket Cycle Mold Rotation Cycle

--- X

(Has special requirements. Refer to “Section 5” for more information.)

Activate/deactivate compensation automatically when you program the move or cycle. Tool diameter must be active.

Elbow Mold Cycle

(No compensation available.)

Programming a Dwell

--- ---

Dwell pauses a running program for a specified length of time, in seconds. Dwell resolution is 0.1 sec. When the operator types 0.0 seconds (infinite dwell), the CNC will hold indefinitely. Press

START to

restart the CNC after an infinite dwell. To program a Dwell using hot keys:

1. In Edit Mode, press

8/DWELL. The DWELL graphic menu prompts for

length of time in seconds.

2. Type the time, and press

ENTER to add Dwell block to the Program

Listing.

To program a Dwell using soft keys:

1. In Edit Mode, press Sub (F8) to display the Secondary soft key functions.

2. Press Dwell (F7) to activate the DWELL graphic menu.

3. Type the time, and press

ENTER to add Dwell block to the Program

Listing.

CNC Programming and Operations Manual

P/N 70000504I - Writing Programs

Programming a Return to Machine Zero

NOTE: The CNC measures all typed coordinates in the Machine Home

graphic menu from Machine Zero. The CNC homes axes one at a time, in the order indicated in the Setup Utility.

A Home block re-establishes a permanent reference position located on the machine. The position is called Machine Zero. Program a Home block using one of the two methods described in Table 4-2.

Table 4-2, Homing Methods

Homing Method Required Action

1. Indicate axes

Activate Machine Home graphic menu. Press required X, Y, Z-axis keys. On each axis selected, machine feeds from the current position to the limit switch, reverses direction and travels to the first detected zero crossing, and sets Machine Zero at that point.

2. Type coordinates

Activate Machine Home graphic menu. For each required axis, highlight the axis entry field and type a coordinate (example: X0, Y-1, Z-4). The machine rapids to the typed coordinate, then feeds to the limit switch, reverses direction and travels to the first detected zero crossing, and sets Machine Zero at that point.

Use Homing Method 1 to execute a homing sequence in feed. Use Homing Method 2 to execute a homing sequence that rapids to the typed coordinate, then initiates the homing sequence.

To activate the Machine Home graphic menu:

1. In the Edit Mode, press Mill (F5) to display the Mill soft keys.

2. Press More (F7) to display the More pop-up menu.

3. Highlight Home and press

ENTER to display the Machine Home

graphic menu.

The method used to set Machine Zero depends on which options the builder installs. Check with the machine builder for detailed information.

CNC Programming and Operations Manual

P/N 70000504I - Writing Programs

Programming Fixture Offsets

NOTE: Presets and SetZero will work with Fixture Offsets.

Refer to Figure 4-2.

Figure 4-2, Fixture Offset Graphic Menu

To program a Fixture Offset:

1. In Edit Mode, press Mill (F5) to display the Mill soft keys.

2. Press More (F7) to display the More pop-up menu.

3. Select Offsets and press

ENTER to display the Fixture Offset graphic

menu.

4. Fill in the labeled entry fields, as follows:

Fixture#

The Fixture-Offset number. Indicates which set of values from the Fixture Offsets Table will be activated or changed. Type a number 1 through 9, corresponding to the Fixture Offsets Table, to activate or change an offset. Type 0 to cancel fixture offsets.

X-offset coordinate. If you do not type a value, the CNC activates the offsets listed in the Fixture Offsets Table for the typed Fixture#. If you do type a value, the CNC applies the typed offset. When the program runs, the CNC updates the Fixture Offsets Table with the specified X offset and clears the previous value. Optional.

Y-offset coordinate. If you do not type a value, the CNC activates the offsets listed in the Fixture Offsets Table for the typed Fixture#. If you do type a value, the CNC applies the typed offset. When the program runs, the CNC updates the Fixture Offsets Table with the specified Y offset and clears the previous value. Optional.

CNC Programming and Operations Manual

P/N 70000504I - Writing Programs

Z-Offset coordinate. If you do not type a value, the CNC activates the offsets listed in the Fixture Offsets Table for the typed Fixture#. If you do type a value, the CNC applies the typed offset. When the program runs, the CNC updates the Fixture Offsets Table with the specified Z offset and clears the previous value. Optional.

To cancel Fixture Offsets:

1. In Edit Mode, press Mill (F5) to display the Mill soft keys.

2. Press More (F7) to display the More pop-up menu.

3. Select Offsets, and press

ENTER to display the Fixture Offset graphic

menu.

4. Select Fixture#. In the highlighted entry field, type 0 to cancel Fixture Offsets. (Do not fill in the other entry fields.)

Fixture Offsets Table

The Fixture Offsets Table, accessed using the Tool Page, contains the typed values for Fixture Offsets 1 through 9. Refer to Figure 4-3.

NOTE: Handwheel and Jog features are available while the Fixture

Offsets Table is active.

Figure 4-3, Fixture Offsets Table

Activating the Fixture Offsets Table

To activate the Fixture Offsets Table:

1. In the Tool Page, press OFFSETS (F1).

CNC Programming and Operations Manual

P/N 70000504I - Writing Programs

Changing Fixture Offsets in the Table

There are three ways to change the values in the table: manually type a value, or calibrate the fixture offset table entry to the machine’s current location (shown on the axis display), or adjust an existing entry.

To change a fixture offset to a manually typed coordinate:

1. Highlight a Fixture Offset (row 1 through 9).

2. Press an axis key (X, Y, or Z).

3. Type a value, and press

To calibrate the fixture offset table entry to the machine’s current location:

1. Highlight a Fixture Offset (row 1 through 9).

2. Press CalibX (F5), CalibY (F6), or CalibZ (F7) to store the current machine position for the selected axis in the table.

To adjust a fixture offset table entry:

1. Highlight a Fixture Offset (row 1 through 9).

2. Press the ABS/INC key, or ALT + E on a keyboard, to display a pop- up message, “Enter axis and adjustment value.”

3. Type the axis to adjust (X, Y, or Z) and the amount of the adjustment. The adjustment value can be positive or negative.

4. Press

ENTER to adjust the value, and display the adjusted value in the

table.

Resetting Absolute Zero (Part Zero)

Absolute Zero is the X0, Y0 position for absolute dimensions. Refer to “Section 1 - CNC Programming Concepts” for information on Absolute Positioning. A SetZero block sets the Absolute Zero Reference of one or more axes to a new position. Use SetZero in one of two ways: to reset X0 Y0 or to preset the current location to typed coordinates.

ENTER to store the value in the table.

In axis presetting, non-zero XY values set the current machine position to the typed coordinates. In axis resetting, X0 and Y0 values set the current machine position as the new Absolute Zero Reference.

When the CNC executes the block, the X and Y values (zero or non-zero) in the graphic menu redefine Absolute Zero.

In Figure 4-4, Executing a SetZero Block, diagram A shows Part Zero and tool position prior to a SetZero block. In this example, the operator programs a SetZero block with the following coordinates: X2, Y-1.

Diagram B shows Part Zero and tool position following the SetZero block. The coordinates at the tool position become X2, Y-1. This, in effect, moves Part Zero, as indicated.

CNC Programming and Operations Manual

P/N 70000504I - Writing Programs

Figure 4-4, Executing a SetZero Block

Change Absolute Zero to cut more than one part with the same moves. Restore the location of the original X0, Y0 reference at the end of the program so that programmed part change positions do not move each time the program runs. Refer to Figure 4-5.

Figure 4-5, Using SetZero in a Program

CNC Programming and Operations Manual

P/N 70000504I - Writing Programs

When an axis entry field (X, Y, or Z) remains blank in a graphic menu, the CNC does not change the position of that axis. Refer to Figure 4-6.

NOTE: In most programs, the Z-axis position does not change.

Changing the Z-axis position changes the Tool #0, Z0 position, which alters all existing tool-length offsets.

Figure 4-6, Set Zero Graphic Menu

To program a SetZero block:

1. In Edit Mode, press Mill (F5) to change the Soft Key labels.

2. Press More (F7) to display the pop-up menu.

3. Position the highlight to select SetZero, and then press Set Program Zero Graphic menu prompts for the absolute coordinates of the machine’s current position.

4. Type the appropriate X, Y, and Z coordinates and press the block to the Program Listing.

Programming a Plane Change

The CNC executes Arc moves and compensates for tool diameters in three different planes (XY, YZ, and XZ). By default, the CNC operates in the XY plane. Program a Plane block to change the CNC’s active plane. Following moves in the XZ or YZ plane, program a second Plane block to return to the XY plane. Refer to “Section 1 - CNC Programming Concepts” for basic information on planes.

A Plane block also changes the active plane of the Program Editor. The Program Editor customizes Arc graphic menus for the active plane.

When a plane block is deleted from the Program Listing, the active plane of the Editor does not change.

ENTER. The

ENTER to add

To program a Plane block using hot keys (the keypad):

1. In Edit Mode, press

9/PLANE. The SET PLANE graphic menu prompts

for plane selection.

2. Press the +/- key to change the selection to the desired plane. Press

ENTER to add the block to the Program Listing.

CNC Programming and Operations Manual

P/N 70000504I - Writing Programs

To program a Plane block using soft keys:

1. In Edit Mode press Mill (F5) to display the Mill soft keys.

2. Press More (F7) to display the More pop-up menu.

3. Highlight Plane, and press prompts for plane selection.

4. Press +/- to change to the desired plane. Press block to the Program Listing.

Programming a Feedrate Change

A Feed block sets the feedrate for Line moves, arcs, and cycles that do not contain specifically programmed feedrates. Feed blocks also set the feedrate for modal moves. Add Feed blocks whenever necessary.

NOTE: A Feed block does not activate the Feed Mode. To program a Feed block from the hot keys (the keypad):

1. In Edit Mode, press

2. Type the required feedrate, and press Program Listing.

To program a Feed block from the soft keys:

1. In Edit Mode, press Mill (F5) to display the Mill soft keys.

2. Press More (F7) to display the More pop-up menu.

3. Highlight Feed, and press menu.

ENTER. The SET PLANE graphic menu

ENTER to add the

4/FEED to display the FEEDRATE graphic menu.

ENTER to add the block to the

ENTER to activate the FEEDRATE graphic

4. Press Save (F10) or

ENTER to add Feed block to the Program Listing.

If the machine has a 4th axis (typically, U) a feedrate can be programmed for the U-axis using the FeedU block. If the U-axis is a rotary axis, the units for the FeedU block are degrees per minute (deg/min); otherwise, the units are the same as in the Feed block.

To program a FeedU block from the soft keys:

1. In Edit, or MDI, press Mill (F5) to display the Mill keys.

2. Press More (F7) to display the More keys

3. Highlight FeedU and press

4. Type the desired value, and press Save (F10) or

ENTER to display the FeedU graphic menu.

ENTER to add the

FeedU block to the program.

CNC Programming and Operations Manual

P/N 70000504I - Writing Programs

Programming a Spindle RPM

If your CNC has a programmable spindle RPM, you can set the RPM in one of the following ways.

• Each tool has an associated RPM entry in the tool page. When a tool

is made active, its associated RPM is used.

• You can use the RPM block in the program. This is especially

necessary when you use more than one spindle speed with a specific tool.

To program an RPM block from the hot keys (the keypad):

1. In Edit Mode, press the

(Decimal/RPM) key to display the Spindle

RPM graphic menu.

2. Type the required spindle RPM and press

ENTER to add the block to

the Program Listing.

To program an RPM block from the soft keys:

1. In Edit Mode, press Mill (F5) to display the Mill soft keys.

2. Press More (F7) to display the More pop-up menu.

3. Highlight RPM and press

ENTER to activate the Spindle RPM graphic

menu.

4. Type the required RPM, and press Save (F10) or

ENTER to add RPM

block to the Program Listing.

CNC Programming and Operations Manual

P/N 70000504I - Writing Programs

Straight Moves

Programming a Rapid Move

Rapid moves run at the CNC’s Rapid rate and save time when positioning for a cut or a canned cycle.

Use Rapid moves to activate/deactivate tool diameter compensation and cutter compensation. Refer to Figure 4-7.

Figure 4-7, Rapid Move Graphic Menu

To program a Rapid move using hot keys (the keypad):

1. In Edit Mode, press

1/RAPID to activate the RAPID (XY) graphic menu.

2. Type the X, Y, and Z coordinates in the appropriate entry fields.

3. Press +/- to set ToolComp (optional) and press

ENTER to highlight

Tool#.

4. Type a tool number (optional), and press

ENTER to add the Rapid

block to the Program Listing.

To program a Rapid move using soft keys:

1. In Edit Mode, press Mill (F5) to display the Mill soft keys.

2. Press Rapid (F2) to activate the RAPID (XY) graphic menu.

3. Type the appropriate values and settings in the labeled entry fields.

CNC Programming and Operations Manual

P/N 70000504I - Writing Programs

Programming a Line Move

Straight line moves run in Feed. Refer to Figure 4-8.

Figure 4-8, Line Move Graphic Menu

To program a Line move using hot keys (the keypad):

1. In Edit Mode, press

2. Type the appropriate values and settings in the labeled entry fields.

To program a Line move using soft keys:

1. In Edit Mode, press Mill (F5) to change the Soft Key labels.

2. Press Line (F3) to display the LINE (XY) graphic menu.

3. Type the appropriate values and settings in the labeled entry fields.

4. With the last entry field highlighted, press the Program Listing.

Programming a Modal Move

A modal move is a straight move executed in the active Rapid or Feed Mode.

To program a Modal move:

1. In Edit Mode, press X, Y, or Z. The MODAL MOVE graphic menu prompts for the X, Y, and Z positions.

2. Type the required positions.

3. From the last field on the graphic menu, press add the modal move block (Xn Yn Zn) to the program.

2/LINE to activate the LINE (XY) graphic menu.

ENTER to add the block to

ENTER or Save (F10) to

NOTE: When using modal moves, be sure the CNC is in the required

Rapid or Line Mode. The CNC executes Line Mode moves in Feed Mode.

CNC Programming and Operations Manual

P/N 70000504I - Writing Programs

Teach Mode (Programming from the Part)

In Teach Mode, the CNC writes program blocks that duplicate manually executed moves. Teach Mode allows you to select endpoints from a part diagram to program a move without knowing the coordinates.

Teach Mode also operates in DRO Mode. To activate the Teach Mode from the Edit screen:

1. Press Teach (F1). The Teach (F1) soft key highlights.

Use Teach Mode to program a Line, Rapid, or Modal move. Refer to

Figure 4-9.

Figure 4-9, Teach Mode Screen

To program a Teach move:

1. In Edit Mode, press Teach (F1) to activate Teach Mode. The display shows the current location.

2. Manually position the machine at the endpoint.

3. Press Rapid (F2), Line (F3), or Modal (F4) to indicate the required move type. The CNC inserts the appropriate block into the listing.

4. Program all required moves in Teach Mode.

5. Press Teach (F1) to deactivate Teach Mode.

CNC Programming and Operations Manual

P/N 70000504I - Writing Programs

Line or Rapid Moves

Using the X, Y, or XY endpoints, the CNC can write Line or Rapid moves. The CNC calculates the missing endpoint(s). Define the move as part of a right triangle with the components identified as in Figure 4-10.

NOSTOP

Figure 4-10, Move Orientation

The CNC can calculate move endpoints, given:

• Angle and radius

• X position and angle

• Y position and angle

• X position and radius

• Y position and radius

The Rapid and Line graphic menus are similar. However, the Rapid graphic menus do not contain CornerRad or Feed entry fields. Use either the Absolute or Incremental Mode.

CNC Programming and Operations Manual

P/N 70000504I - Writing Programs

Programming a Move Using XY Location, Radii, or Angles

To program a move using a Line or Rapid block:

1. In Edit Mode, press Mill (F5) and select either Rapid (F2) or Line (F3).

– or –

In Edit Mode, press

1/RAPID or 2/LINE to display the RAPID (XY) or

LINE (XY) graphic menu.

2. Press More. . . (F4) to display the Template pop-up menu. Refer to Figure 4-11.

Figure 4-11, Rapid/Line Template Pop-up Menu

3. Highlight the appropriate template, and press

ENTER to display the

graphic menu.

4. Type the required values/settings in the entry fields.

CNC Programming and Operations Manual

(Neg

)

(

)

P/N 70000504I - Writing Programs

Arcs

Selecting the Plane for an Arc

Refer to “Section 1 - CNC Programming Concepts” for information on planes and Arc directions. The CNC executes Arcs in the XY plane by default. For an Arc in the XZ or YZ plane, program the plane change before the Arc move. The plane change customizes the Arc graphic menus for the required plane.

The graphic menus for moves in the XY, XZ, and YZ planes contain the same entry fields. Entry fields for selected plane positions require a value.

After a move in the XZ or YZ plane, return the CNC to the XY plane. NOTE: To activate a new plane in the Program Editor, program a plane

change block.

Program Arc moves:

 Using the endpoint and radius  Using the center and endpoint  Using the center and angle

Programming an Arc Using an Endpoint and Radius

To define the Endpoint - Radius Arc, type the direction of the Arc, the endpoint, and the radius. The CNC cuts an Arc of the specified radius from the current position to the endpoint. You must correctly define the modal endpoint coordinates in the Absolute or Incremental Mode.

In the XY plane, if the Z-axis starting and end points differ, the arc is a helix.

Two Arcs can intersect any two points: an Arc with an included angle less than 180 degrees and an Arc with an included angle greater than 180 degrees. Refer to Figure 4-12.

IncludedAngle

Less Than 180 De

Positive Radius V alue

Sta Point

ees

End

Point

Start Point

IncludedAngle

eaterThan 180 De

ative Radius Value

ees

End

Point

Figure 4-12, Endpoint Radius Arc Types

CNC Programming and Operations Manual

P/N 70000504I - Writing Programs

To program an Arc with an included angle less than 180 degrees, type a positive radius value. To program an Arc with an included angle greater than 180 degrees, type a negative radius value. The CNC selects which Arc center to use, based on the sign of the typed value.

To program an Arc using an endpoint and radius, using hot keys (the keypad):

1. In Edit Mode, press

3/ARC. The ARC (END POINT - RADIUS) graphic

menu prompts for labeled values.

2. Fill in the entry fields as labeled.

To program an Arc using an endpoint and radius, using soft keys:

1. In Edit Mode, press Mill (F5) to display the Mill secondary soft keys.

2. Press Arc (F4) to display the ARC (END POINT - RADIUS) graphic menu. Refer to Figure 4-13.

Figure 4-13, ARC (END POINT - RADIUS) Graphic Menu

3. Fill in the ARC (END POINT - RADIUS) entry fields: Direction Specifies a clockwise (Cw) or counterclockwise

(Ccw) direction. Press +/- to toggle the setting. Selection required.

X The X coordinate of the Arc endpoint. Value

required.

Y The Y coordinate of the Arc endpoint. Value

required.

Z The Z coordinate of the endpoint. Optional. Radius The radius of the Arc. Value required (positive or

negative).

CornerRad Corner radius setting. Optional. (Refer to

“Section 1 - CNC Programming Concepts” for details.)

Feed Feedrate. Optional. Tool# Active tool. Optional.

CNC Programming and Operations Manual

P/N 70000504I - Writing Programs

Programming an Arc Using the Center and Endpoint

NOTE: Use Center and Endpoint Arcs to cut helical threads.

To define the Center - Endpoint Arc, type the endpoint, arc center, and direction. The CNC cuts an Arc from the current position to the end point.

In Absolute Mode, the CNC measures the Arc center and endpoint from Absolute Zero. In Incremental Mode, the CNC measures the Arc center and end point from the starting position of the arc.

NOTE: Ensure that the required Absolute or Incremental Mode is active. When the Z-axis start and end points differ in the XY plane, the Arc is a

helix. The Revs value determines the number of rotations used to machine the helix.

The CNC calculates the radius from the specified starting point and Arc center. Therefore, the endpoint must lie along the Arc’s path. If the endpoint does not lie along the Arc’s path, the CNC will adjust the center or end point. Configure whether the CNC will adjust the center or endpoint in the Setup Utility. Endpoint is preferred. The machine builder sets the maximum arc circle center adjustment in the Setup Utility. If the error exceeds the setup tolerance, the CNC generates an error message.

To program a Center - End Point Arc using hot keys (the keypad):

1. In Edit Mode, press 3/

ARC to display the ARC (CENTER – END

POINT) graphic menu. Refer to Figure 4-14.

Figure 4-14, ARC (CENTER – END POINT) Graphic Menu

2. Press More... (F4) to display the Arc template pop-up menu. Refer to Figure 4-15, Arc Template Pop-Up Menu.

3. Highlight the Center – End Point template and press the

ARC (CENTER – END POINT) graphic menu.

ENTER to display

4. Type the required values or settings in the entry fields.

CNC Programming and Operations Manual

P/N 70000504I - Writing Programs

To program a Center – End Point Arc using soft keys:

1. In Edit Mode, press Mill (F5) to display the

Mill secondary soft keys.

2. Press Arc (F4) to display the ARC (END POINT - RADIUS) graphic menu.

3. Press More... (F4) to display the Arc Template pop-up menu. (Refer to Figure 4-15).

Figure 4-15, Arc Template Pop-Up Menu

4. Highlight the Center – End Point template and press

ENTER. The

ARC (CENTER – END POINT) graphic menu prompts for the labeled

values.

5. Type the required values or setting in the following labeled entry fields:

Direction Allows you to select a clockwise (Cw) or

counterclockwise (Ccw) direction. Press +/- to toggle the setting. Selection required.

X The X coordinate of the Arc end point. Optional. Y The Y coordinate of the Arc end point. Optional. Z The Z coordinate of the Arc end point. Optional. XCenter The X coordinate of the Arc center. Value required. YCenter The Y coordinate of the Arc center. Value required. Revs Number of revolutions from start position to endpoint.

Optional.

CornerRad Corner radius setting. Optional. (Refer “Section 1 -

CNC Programming Concepts” for details.)

Feed Feedrate. Optional. Tool# Active tool. Optional.

CNC Programming and Operations Manual

(Pr

)

(

)

(Pr

)

(

)

P/N 70000504I - Writing Programs

Programming an Arc Using the Center and the Included Angle

To define the Center - Angle Arc, type the arc center and the included angle. The CNC cuts the Arc from the present position until the Arc travels the specified number of degrees. The CNC calculates the radius, which is the distance between the start position and the center point.

Specify the appropriate Absolute or Incremental Mode for the angle and center point. Refer to Figure 4-16 and Figure 4-17.

The direction (Cw/Ccw) of the Arc and the sign (+/-) of the angle control the path of the tool.

If the Z-axis starting and end points differ, the Arc will be a helix.

bsolute Position

Cw Tool Path

Ccw Tool Path

CenterPoint

bsolute Position

Figure 4-16, Absolute Mode, Center - Angle Arc

Incremental Position

CenterPoint

Incremental Position

bsoluteAngle

Refe

StartingPoint

esent Position

Ccw Tool Path

StartingPoint

esent Position

Cw Tool Path

ence

Figure 4-17, Incremental Mode, Center - Angle Arc

CNC Programming and Operations Manual

P/N 70000504I - Writing Programs

Refer to Figure 4-18.

Figure 4-18, Arc (Center - Angle) Graphic Menu

To program an Arc using the center and the included angle using hot keys (the keypad):

1. In Edit Mode, press

3/ARC to display the ARC (ENDPOINT - RADIUS)

graphic menu.

2. Press More... (F4) to display the Arc Template pop-up menu. (Refer to Figure 4-15, Arc Template Pop-Up Menu.)

3. Highlight the Center - Angle template and press

ENTER to display the

ARC (CENTER - ANGLE) graphic menu.

4. Type the required values and settings in the entry fields.

To program an Arc using the center and the included angle using soft keys:

1. In Edit Mode, press Mill (F5) to activate the Mill secondary soft keys.

2. Press Arc (F4) to display the ARC (END POINT - RADIUS) graphic menu.

3. Press More... (F4) to display the Arc template pop-up menu. Refer to Figure 4-15, Arc Template Pop-Up Menu.

4. Highlight the Center - Angle template and press

ENTER to display the

ARC (CENTER - ANGLE) graphic menu.

5. Fill in the ARC (CENTER - ANGLE) entry fields: Direction Specifies a clockwise (Cw) or counterclockwise (Ccw)

direction. Press +/- to toggle the setting. Selection required.

XCenter The X coordinate of the Arc’s center. Value required. YCenter The Y coordinate of the Arc’s center. Value required. Angle Included angle of the Arc. Value required. Z The Z coordinate of the Arc endpoint. Optional. CornerRad Corner radius setting. Optional. (Refer to “Section 1 -

CNC Programming Concepts” for details.)

Feed Feedrate. Optional. Tool# Active tool. Optional.

CNC Programming and Operations Manual

P/N 70000504I - Writing Programs

Programming M-Code Blocks

The CNC supports M-Code functions. Enable available M-Codes at installation. Refer to the machine builder’s technical data to determine which M-Codes are available.

Some programmed events initiate the same functions activated using M-Codes. Refer to Table 4-3 for a list of the most commonly used M-Code functions.

Table 4-3, M-Code Functions

M-Code

Programmed Event

M02 EndMain block. M03

Activation of a tool that lists a FWD spindle direction on the Tool Page.

M04

Activation of a tool that lists a REV spindle direction on the Tool Page.

M05

Activation of a tool block (to allow a tool change). Activation of a tool that contains a Tool Page spindle direction OFF.

M03, M05, M04

M08

Execution of Tapping Cycle.

Activation of a tool with coolant

ON listed on the Tool Page.

Standard Function Usage

(ref. EIA Standard RS 274-D)

Stops spindle and coolant. Start CW spindle rotation.

Start CCW spindle rotation.

Stop spindle in normal manner.

Start CW spindle rotation, stop spindle then start CCW spindle rotation.

Turn coolant pump ON.

M09

Activation of a tool with coolant

Turn coolant pump OFF.

OFF listed on the Tool Page.

To program an MCode block:

1. In Edit Mode, press MCode (F8). The Graphic menu prompts for the MCode number and X, Y, Z values.

2. Type the values and press Save (F10) or

ENTER to add MCode block

to the program.

CNC Programming and Operations Manual

P/N 70000504I - Writing Programs

Dry Run M-Codes

In Dry Run Mode, the machine axes (X, Y, and Z) move through the program without cutting into the work. The CNC disables coolant operation and the work may or may not be placed on the table.

Activate Dry Run Mode with M-Codes 105 and 106. Deactivate it with M107. Refer to Table 4-4. Dry Run feedrates are set in the Setup Utility. They are often set at greater speeds than conventional feedrates. You can set them at any desired rate. Refer to the 3000M CNC Setup Utility Manual, P/N 70000499, for details.

Table 4-4, Dry Run Mode M-Codes

M-Code Function Description

M105 Dry Run Mode ON,

M106 Dry Run Mode ON,

M107

U-Axis Synchronization M-Codes

For systems that have a U-axis, the U-axis can be synchronized with XYZ or unsynchronized. The following M-codes are used to specify U-axis synchronization in Manual Data Input (MDI) or in a program. The builder sets the default configuration. Refer to Table 4-5.

Table 4-5, U-Axis Synchronization M-Codes

M-Code Function Description

M900

all axes

no Z-axis

Cancel Dry Run Mode

Activate 4

(U) axis

synchronization

Enables machine Z Dry Run Mode. Program runs at dry run feedrates specified in the Setup Utility.

Enables machine Dry Run Mode. Program runs at dry run feedrates specified in the Setup Utility, without moving the Z-axis.

Cancels active Dry Run Mode.

Axes to be synchronized must also be programmed. Example: Mcode 9000 U will synchronize the U-axis with XYZ feedrate. All moves feedrates will be vectored.

M901

Deactivate 4 axis synchronization

(U)

Indicate axis to deactivate synchronization. Example: Mcode 9001 U will unsynchronize the U-axis with XYZ feedrate.

CNC Programming and Operations Manual

P/N 70000504I - Programming Canned Cycles, Ellipses, and Spirals

Section 5 - Programming Canned Cycles, Ellipses, and Spirals

Drilling Cycles

Drill cycles simplify the programming required for repetitive drilling, boring, and tapping operations. Select specific drill cycles from the Program Editor’s Drill (F3) pop-up menu:

NOTE: Program all blocks by filling in the entry fields of a Graphic Menu.

 Basic (drill cycle)  Pecking  Boring  Chip Break  Tapping  Drilling Off  Pattern  Bolt Hole  Thread Mill  ZMode

Drill cycles are modal. When the CNC encounters a block for any type of Drill cycle, it executes that cycle at the endpoint of each subsequent move until it encounters a DrillOff block. To change drill cycle parameters between moves, program a new drill block.

Program a ZMode block to switch the operation between two-axes and three-axes as needed in a program. To program a ZMode block, select

ZMode from the Drill (F3) pop-up menu and then press +/- key to select: TwoAxAuto, TwoAxStep, or ThreeAxes.

If the CNC is in ThreeAxes mode and a TwoAxStep or TwoAxAuto block is ran, the operator is prompted to disengage the Z-axis and, subsequently, to position the Z-axis manually when needed. When in TwoAxStep block, the machine will stop on every move, as when drilling. When in a TwoAxAuto block, as when milling a contour, the motion is continuous until the CNC sees a ZMove.

If the CNC is in TwoAxAuto or TwoAxStep mode and a ThreeAxes block is ran, the operator is prompted to re-engage the Z-axis. To re-engage the Z-axis drive system, lift the quill handle until you feel the drive assembly become seated, then tighten the quick release knob. Once the Z-axis is re-engaged, the operator can jog the Z-axis to the homing mark on the front of the Z-axis drive system and (if needed) press

START to perform a Homing sequence or Manual (F4) to cancel the

Homing sequence. Another press of the

START key allows the program to

continue to run normally.

CNC Programming and Operations Manual

P/N 70000504I - Programming Canned Cycles, Ellipses, and Spirals

Basic Drill Cycle

The Basic Drill Cycle is a modal operation. When the CNC receives a BasicDrill command, it performs the drilling operation at the endpoint of every subsequent block until it receives a Drilling Off block. To change Basic Drilling dimensions cancel the current cycle and program a new cycle.

During the cycle, the tool rapids to the StartHgt, then Z feeds to ZDepth. To provide clearance for the next move, at the end of the cycle, the tool rapids to ReturnHgt.

Z-axis depth can be changed by placing a new Z depth on the same line as the X- and/or Y-axis location of the hole you want the new depth applied. A Z address on a line of its own will cause the control to drill the new depth at the current location.

Program a DrillOff block to deactivate the cycle. You can program any number of patterns and moves before turning off the cycle.

To program a BasicDrill block:

1. In Edit mode, press Drill (F3) to display the Drill cycle pop-up menu.

2. Highlight Basic, and press

ENTER to display the BASIC DRILLING

Graphic Menu. Refer to Figure 5-1.

Figure 5-1, BASIC DRILLING Graphic Menu

3. Enter the required values and settings in the entry fields. With the last entry field highlighted, press

ENTER. The display clears and the CNC

adds the BasicDrill block to the program listing.

4. Program subsequent moves to position the tool at the required drilling location(s). The CNC will drill a hole at the endpoint of every move.

5. After programming the last drill move, press Drill (F3) to display the Drill cycle pop-up menu.

6. Highlight Drilling Off, and press

ENTER to cancel the Drilling Mode.

CNC Programming and Operations Manual

P/N 70000504I - Programming Canned Cycles, Ellipses, and Spirals

BASIC DRILLING entry fields:

ZDepth The absolute depth of the finished hole. (Required)

NOTE: ZDepth must be lower than StartHgt. StartHgt is 0.100

inches (2.0 mm) above the work surface.

StartHgt The absolute Z position the CNC rapids to before

feeding into the work. (Required)

ReturnHgt The absolute position to which the tool returns at

the end of the cycle. (Optional)

Feed Feedrate. (Optional) Tool# Active tool. (Optional)

Peck Drilling Cycle

Peck drilling is a modal operation. When the CNC receives a PeckDrill command, it peck-drills at the endpoint of every subsequent block until it receives a Drilling Off block. To change Peck Drilling dimensions, cancel the current PeckDrill cycle and program a new cycle.

The cycle starts when the CNC is in position. The tool rapids to the Z start height (StartHgt); feeds to the Peck depth; then rapids back to the StartHgt. This cycle repeats until the tool reaches ZDepth. At the end of the cycle, the tool rapids to the ReturnHgt to provide clearance for the next move.

To program a Peck Drilling cycle:

1. In Edit mode, press Drill (F3) to display the Drill cycle pop-up menu.

2. Highlight Pecking, and press

ENTER to display the PECK DRILLING

Graphic Menu. Refer to Figure 5-2.

Figure 5-2, PECK DRILLING Graphic Menu

3. Enter the required values and settings in the entry fields. With the last entry field highlighted, press

ENTER. The Display clears and the CNC

adds the PeckDrill block to the program listing.

4. Program subsequent moves to position the tool at the required drilling location(s). The CNC will drill a hole at the endpoint of every move.

CNC Programming and Operations Manual

P/N 70000504I - Programming Canned Cycles, Ellipses, and Spirals

5. After programming the last drill move, press Drill (F3) to display the

Drill cycle pop-up menu.

Boring Cycle

6. Highlight Drilling Off, and press

ENTER to cancel the Drilling Mode.

PECK DRILLING entry fields:

ZDepth Absolute depth of the finished hole. (Required) NOTE: ZDepth must be lower than StartHgt. StartHgt is 0.100

inches (2.0 mm) above the work surface.

StartHgt Absolute Z position the CNC rapids to before

feeding into work. (Required)

ReturnHgt Absolute position the tool returns to at the end of

the cycle. (Optional)

Peck Depth drilled in each peck. (Required) Tool# Active tool. (Optional)

Boring is a modal operation. When the CNC encounters a Boring block, it executes a Boring Cycle at the endpoint of every subsequent move until it sees a Drilling Off block. To change Boring Cycle dimensions between moves, deactivate the cycle and program a new boring block.

The cycle starts when the CNC is in position. The tool rapids to the StartHgt, feeds to ZDepth, and then feeds back to StartHgt. At the end of the cycle, the tool moves to ReturnHgt to provide clearance for the next move.

When running a Dwell block, the CNC pauses at ZDepth for the indicated time period (in seconds). Dwell resolution is 0.1 sec. When you enter

0.0 sec., the CNC dwells until manually restarted.

To program a Boring cycle:

1. In Edit mode, press Drill (F3) to display the Drill cycle pop-up menu.

2. Highlight Boring, and press

ENTER to display the BORING CYCLE

Graphic Menu. Refer to Figure 5-3.

Figure 5-3, BORING CYCLE Graphic Menu

CNC Programming and Operations Manual

P/N 70000504I - Programming Canned Cycles, Ellipses, and Spirals

BORING CYCLE entry fields:

ZDepth Absolute depth of the finished hole. (Required) NOTE: ZDepth must be lower than StartHgt. StartHgt is 0.100

inches (2.0 MM) above the work surface.

StartHgt Absolute Z position the CNC rapids to before

feeding into work. (Required)

ReturnHgt Absolute position to which the tool returns at the

end of the cycle. (Optional)

Dwell Length of time for pause at ZDepth. (Optional) Feed Feedrate. (Optional) Tool# Active tool. (Optional)

3. Enter the required values and settings in the entry fields. With the last entry field highlighted, press

ENTER. The display clears and the CNC

adds Boring block to the program listing.

4. Program subsequent moves to position the work at the required boring locations. The CNC executes the Boring Cycle at the endpoint of every move.

5. After programming the last boring position, press Drill (F3) to display

6. Highlight Drilling Off, and press

Chip Break Cycle

The Chip Break Cycle is modal. Once the CNC encounters a ChipBreak block, it executes the Chip Break Cycle at the endpoint of each block until it sees a Drilling Off block. To change Chip Break values between moves, deactivate the cycle and program a new one.

The cycle starts when the CNC is in position. The tool rapids to the StartHgt, feeds to the FirstPeck, retracts 0.02 inches [0.4 mm (default value)], then feeds to the next peck. Retract moves occur at the end of each peck in order to break the chip. This cycle repeats until the tool reaches ZDepth. At the end of the cycle, the tool moves to ReturnHgt to provide clearance for the next move.

Enter a PeckDecr value to decrement the depth of each peck by the specified amount. The MinPeck sets the minimum peck the cycle can decrement. A ChipBrkInc is the size of the retract move that breaks the chip.

Peck to the RetractDep, retract to the StartHgt, and then peck to the next RetractDep increment. The first full retract occurs one RetractDep increment after the first peck.

the Drill cycle pop-up menu.

ENTER to cancel the cycle.

CNC Programming and Operations Manual

P/N 70000504I - Programming Canned Cycles, Ellipses, and Spirals

To program a Chip Break cycle:

1. In Edit Mode, press Drill (F3) to display the Drill cycle pop-up menu.

2. Highlight Chip Break, and press

ENTER to display the CHIP

BREAKING CYCLE Graphic Menu. Refer to Figure 5-4.

Figure 5-4, CHIP BREAKING CYCLE Graphic Menu

CHIP BREAKING CYCLE entry fields:

ZDepth Absolute depth of the finished hole. (Required) NOTE: ZDepth must be lower than StartHgt. StartHgt is 0.100

inches (2.0 mm) above the work surface.

StartHgt Absolute Z position to which the CNC rapids before

feeding into work. (Required)

ReturnHgt Absolute position to which the tool returns at the

end of the cycle. (Optional)

FirstPeck Absolute depth drilled in each peck. (Required) PeckDecr Amount to subtract from previous peck (positive

dimension). (Required)

MinPeck Smallest peck allowed. (Required) ChipBrkInc Size of chip break retract. (Optional) RetractDep Z increment before full retract. (Optional) Tool# Active tool. (Optional)

3. Enter the required values and settings in the entry fields. entry field highlighted, press

ENTER. The display clears and the CNC

With the last

adds the Chip Break block to the program listing.

4. Program the drilling location(s). The CNC will drill a hole at the endpoint of every move until it receives the Drilling Off command.

5. Program the Drilling Off command. After programming the last drill move, press Drill (F3) to display the Drill cycle pop-up menu.

6. Highlight Drilling Off, and press

ENTER to add the DrillOff block to

the program Listing.

CNC Programming and Operations Manual

P/N 70000504I - Programming Canned Cycles, Ellipses, and Spirals

Tapping Cycle

The Tapping Cycle is available only on machines equipped with spindle RPM control and M-Codes (M3, M4, and M5).

In order for the cycle to operate, you must enter Spindle RPM value for the active tool on the Tool Page. During execution, the CNC uses the Spindle RPM value from the Tool Page and the programmed threads per inch (or pitch) value from the block to calculate the proper feedrate for tapping.

When the cycle, runs the CNC rapids to the StartHgt and feeds to the ZDepth. The spindle stops and reverses direction to retract the tool from the hole. At ReturnHgt, the spindle stops and changes back to the original direction in preparation for the next programmed move.

Use the Tapping Cycle with any available pattern. A Drilling Off block cancels the cycle.

NOTE: The system supports spindle FWD, REV, OFF (M3, M4, M5),

and spindle RPM control. At machine setup the machine builder determines which M-Codes to install.

To program a Tapping block:

1. In Edit mode, press Drill (F3) to display the Drill cycle pop-up menu.

2. Highlight Tapping, and press

ENTER to display the TAPPING CYCLE

Graphic Menu. Refer to Figure 5-5.

Figure 5-5, Tapping Cycle Graphic Menu

TAPPING CYCLE entry fields:

ZDepth Absolute depth of the tapped threads. (Required) NOTE: ZDepth must be lower than StartHgt. StartHgt is 0.100

inches (2.0 mm) above the work surface.

StartHgt Absolute Z position to which the CNC rapids before

feeding into work. (Required)

ReturnHgt Absolute position to which the tool returns at the

end of the cycle. (Optional)

CNC Programming and Operations Manual

P/N 70000504I - Programming Canned Cycles, Ellipses, and Spirals

TPIorLead TPI in Inch or Lead in millimeters. (Required) Tool# Active tool. (Optional) Dwell Length of time for pause at top of hole and at

ZDepth. (Optional)

3. Enter the required settings and values in the entry fields. With the last entry field highlighted, press

ENTER to clear the display and add the

new tapping cycle block to the program listing.

4. Program subsequent moves to position the location of the tapped holes. The CNC will tap a hole at the endpoint of every move until it receives a Drilling Off command.

5. To program a Drilling Off block, press Drill (F3) to display the Drill cycle pop-up menu.

Drill Pattern

6. Highlight Drilling Off, and press

ENTER to display the Drill Off block

in the program listing.

The Pattern Cycle instructs the CNC to execute a pattern of regularly spaced moves. Locate a Pattern Cycle between a Drill Cycle and a DrillOff block. The CNC executes the Drill Cycle at every endpoint in the pattern.

In a Pattern Cycle, enter a size, location, spacing, Tool #, and rotation angle of the pattern.

To program a Drill Pattern cycle:

1. In Edit Mode, press Drill (F3) to display the Drill cycle pop-up menu.

2. Select Pattern from the Drill pop-up menu, and press

ENTER to

display the PATTERN DRILL Graphic Menu. Refer to Figure 5-6.

Figure 5-6, Pattern Drill Graphic Menu

PATTERN DRILL entry fields:

X X coordinate of corner hole. If no entry made, CNC

puts corner hole at present location. (Optional)

Y Y coordinate of corner hole. If no entry made, CNC

puts corner hole at present location. (Optional)

CNC Programming and Operations Manual

P/N 70000504I - Programming Canned Cycles, Ellipses, and Spirals

#XHoles Number of rows that lie along the X-axis. Must enter

value greater than 0. (Required)

#YHoles Number of rows that lie along the Y-axis. Must enter

value greater than 0. (Required)

NOTE: Enter 1 in either the #XHoles or the #YHoles field to drill a

single row or column.

Xincr X-axis increment (spacing) of holes. (Required) Yincr Y-axis increment (spacing) of holes. (Required) Angle This value rotates the pattern. The XY corner hole is

the pivot, and the rotation angle is the number of degrees counterclockwise from the X-axis or 3 o’clock position.

NOTE: Use a Drilling Off block to cancel cycle.

3. Enter the required values and settings in the entry fields.

Bolt Hole Pattern

The Bolt Hole Cycle instructs the CNC to run a series of moves with endpoints that form a circular pattern. At each of these endpoints, you can run a previously programmed Drill Cycle.

You should first program a Drill Cycle to describe the hole being drilled. Then follow the Drill Cycle by one or more moves, patterns, or Bolt Hole cycles to position the CNC for the Drill Cycle. A DrillOff block cancels the cycle.

To program a Bolt Hole Cycle:

1. In Edit Mode, press Drill (F3) to display a pop-up menu.

2. Select Bolt Hole from the pop-up menu, and press

ENTER to display

the BOLTHOLE DRILL Graphic Menu. Refer to Figure 5-7.

Figure 5-7, BOLTHOLE DRILL Graphic Menu

CNC Programming and Operations Manual

P/N 70000504I - Programming Canned Cycles, Ellipses, and Spirals

3. Enter the following required values and settings in the BOLTHOLE

DRILL entry fields: XCenter Absolute X center of the bolt hole pattern. If no

entry is made, the CNC puts the center of the Bolt Hole pattern at X0. (Required)

YCenter Absolute Y center of the bolt hole pattern. If no

entry is made, the CNC puts the center of the Bolt Hole pattern at Y0. (Required)

NOTE: Use absolute center point coordinates whenever possible. #Holes Number of equally spaced holes in the circular

pattern. (Required)

Diameter Diameter of the circular pattern. (Required) StartAngle The number of degrees (from the 3 o’clock

position) to the first hole. (Required)

EndAngle The number of degrees (from the 3 o’clock

position) to the last hole. (Optional)

IndexAngle The number of degrees that the 3 o’clock reference

position rotates around the center (rotates entire pattern). (Optional)

NOTE: Use a Drilling Off block to cancel the cycle.

CNC Programming and Operations Manual

P/N 70000504I - Programming Canned Cycles, Ellipses, and Spirals

Thread Milling Cycle

WARNING: The first move in this cycle is a rapid move to the center of

the thread before moving the Z-axis. Make sure the tool is properly located before calling up this cycle.

Thread Milling Cycle simplifies the programming required to mill a thread. Use the thread milling for cutting inside or outside threads. It will cut either Inch or MM, left or right hand, and Z movement up or down. A single tooth or multi-toothed tool may be used. Start can be at the top or bottom of the hole or boss. Tool Length Offset is set the same as with any other tool or operation. A tool diameter also has to be set in the tool table, as cutter compensation is built into this cycle (cutter compensation is not allowed during the use of this cycle). The tool must be positioned at center of hole or boss, or the parameters for XCenter and YCenter must be specified in the cycle.

XCenter, YCenter, ArcInRad, StockAmt, Passes, RoughFeed, FinFeed, and TaperAng are all optional Input; all other parameters must

be programmed. If the feed rates are not programmed, the CNC will use last feed rate used.

In a tapered thread the Major Diameter is always the major diameter of thread where the ZStart is set. Inside diameter is at finished depth and outside diameter is the diameter of boss.

To program a Thread Milling Cycle:

1. In Edit Mode, press Drill (F3) to display a pop-up menu.

2. Select Thread Mill from the pop-up menu, and press

ENTER to display

the Thread Mill Graphic Menu. Refer to Figure 5-8.

Figure 5-8, Thread Mill Graphic Menu

CNC Programming and Operations Manual

P/N 70000504I - Programming Canned Cycles, Ellipses, and Spirals

3. Enter the following required values and settings in the Thread Mill entry fields:

XCenter Absolute X coordinate of the center of the thread.

If no coordinate is entered, the CNC puts the center of thread as the current tool position. (Optional)

YCenter Absolute Y coordinate of the center of the thread.

If no coordinate is entered, the CNC puts the center of the thread as the current tool position. (Optional)

ZFinish Absolute Z position where the thread cut will finish.

This can be above or below the start position depending on the direction of the thread cut, up or down. (Required)

ZStart Absolute Z position where the thread cut starts.

This can be above or below the finish position depending on the direction of the thread cut, up or down. If not set, the cycle will use the current Z tool position. (Optional)

ZSafePosn An Absolute safe Z position above the part for rapid

moves in X and/or Y. (Required) WARNING: ZSafePosn must be above the part to

avoid a crash while positioning.

MajorDia Major thread diameter. For a tapered thread, it will

be the major diameter at the Z start position. If you have a tapered hole and you start at the top and cut down, you would have a different major diameter than if you started at the bottom and cut up. (Required)

+ –

Value cuts in the CW direction Value cuts in the CCW direction

ThdDepth Depth of thread. The incremental depth of thread

on one side: (Required)

+ –

Value is inside thread Value is outside thread

TPIorLead Threads per inch (TPI) or lead of thread.

(Required) NOTE: The minimum number of threads per inch

is “1”

CNC Programming and Operations Manual

P/N 70000504I - Programming Canned Cycles, Ellipses, and Spirals

ArcInRad Size of radius arcing into start of thread. (Optional)

NOTE: If ArcInRad is a positive value or not set and the thread is “inside,” the cycle will

always return to the center between passes. If ArcInRad is a negative value, the cutter will move to the start or end point that

is closest to the center if inside thread, and farthest away from center if outside thread.

If ArcInRad is not specified and the thread is “outside,” the cutter will back away from the largest diameter by an amount equal to the thread depth.

StockAmt Amount to leave for a finish pass after the roughing

passes. (Optional)

Passes Number of roughing cuts to be taken. (Optional)

NOTE: If StockAmt is not set or set to zero and Passes is 1 or 0, the cycle will make

just one pass at the full depth.. If StockAmt is set to greater than zero and Passes is 1 or 0, the cycle will make

just one pass at the stock depth and one pass at full thread depth. If Passes is set to a negative number, all non-cutting positioning moves will be

rapid.

RoughFeed Feedrate for roughing. (If not set, the cycle will use

the current active feedrate.) (Optional)

FinFeed Feedrate for the finish pass. (If not set, the cycle

will use the current active feedrate.) (Optional)

TaperAng Angle on one side of the thread (not the included

angle). The angle is measured from the right side going counter clockwise with a positive number and clockwise with a negative number. A straight pipe tape with an inside cut would be -1.7833. If not set, then the thread is straight. (Optional)

If X and Y are not programmed, position tool center of the thread before calling the “Thread Mill” cycle:

• X and Y will rapid to the starting position of the thread.

• Z will rapid to the safe height specified in ZSafePosn.

• The Z axis will feed down to the start cut position ZStart. This could

be above or below the Z position specified in the ZFinish position.

• Depending on what is in the ArcInRad parameter, the tool will arc into the first cut position.

CNC Programming and Operations Manual

P/N 70000504I - Programming Canned Cycles, Ellipses, and Spirals

• Spiral up or down, depending on the difference between ZFinish and ZStart and go counterclockwise or clockwise depending if MajorDia

is plus or minus.

• Then arc-out and feed to the thread center for inside threads, or a safe distance away from the thread for outside threads depending on the value in ArcInRad.

• Then feed back to the ZStart height.

• Then feed X and Y to the next depth of cut. The depth of each

roughing pass will be the thread depth specified in the ThdDepth parameter minus the stock amount specified in the StockAmt parameter, divided by the number of roughing passes specified in the Passes parameter.

• The cycle repeats this process until the final finish pass.

• It will then cut the thread at the full thread major diameter.

When cutting a tapered on an inside thread, care should be taken. An error will be generated if the diameter on the small end of the taper becomes too small for the tool to fit along with arc in and out moves. Not entering an arc-in value in the ArcInRad parameter will allow the cycle to move to the center of the hole for maximum clearance.

CNC Programming and Operations Manual

P/N 70000504I - Programming Canned Cycles, Ellipses, and Spirals

Sample Thread Program

This program will cut an 8 TPI thread starting at 0.1 above the hole. The major diameter of the thread is 1 inch. It will take 2 roughing cuts and 1 finish cut with a 0.625 cutter.

Dim Abs Tool# 1 Rapid X 1.0000 Y 1.0000 Rapid Z 0.1000 ThreadMill Finish -1.0 ZStart 0.1 ZSafePosn .5 MajorDia 1.0

ThdDepth .0625 TPIorLead 8 ArcInRad 0.1 StockAmt 0.002 Passes 2 RoughFeed 20.0

FinFeed 5.0 Rapid Z 5.0000 EndMain

The tool will spiral down the thread pitch of 8 threads per inch, finishing at a depth of –1. The starting height is 0.1, the safe rapid Z height is 0.5, the major thread diameter is 1 inch, and depth of thread is 0.0625. The arc-in radius is 0.1 and the stock amount for the finish pass is 0.002. The rough feedrate is 20.0 and the finish feedrate is 5.0.

NOTE: If you would like all non-cutting positioning moves to be rapid,

set Passes to a negative number. The idea is to initially set Passes as a positive number and after proving out the program, change it to a negative number for faster production. If you only need one pass to size and you want the positioning moves to be rapid, set Passes to -1.

CNC Programming and Operations Manual

P/N 70000504I - Programming Canned Cycles, Ellipses, and Spirals

Pocket Cycles

NOTE: Program all blocks by filling in the entry fields of a Graphic Menu.

Pocket canned cycles simplify the programming of repetitive moves required to mill out pockets. Select the pocket-canned cycles from the Program Editor Pocket (F4) pop-up menu. Refer to Figure 5-9.

NOTE: Programming a Tool# in a pocket cycle automatically activates

the necessary tool compensation for that cycle.

Face Rect. Profile Circ. Profile

Rectangular

Circular

Frame

Hole

IRRegular Mold Rotation Elbow Milling

Islands

POCKETPU

Figure 5-9, Pocket Pop-up Menu

Select specific pocket cycles from the Program Editor’s Pocket (F4) pop- up menu:

 Facing Cycle  Rectangular Profile Cycle  Circular Profile Cycle  Rectangular Pocket Cycle  Circular Pocket Cycle  Frame Pocket Cycle  Hole – Mill Cycle  Irregular Pocket Cycle  Mold Rotation  Elbow Milling Cycle  Pockets with Islands

CNC Programming and Operations Manual

P/N 70000504I - Programming Canned Cycles, Ellipses, and Spirals

Facing Cycle

Facing cycles simplify the programming required to face the surface of a part.

Execution begins one tool radius from the start point. The selected stepover determines the approach axes.

NOTE: A ZDepth entry is not necessary if you program only one level

plus finish stock.

Facing cycles can start in any corner of the surface and cut in any direction, depending on the sign (+/-) of the Length and Width values. Program a slightly oversize Length and Width to ensure complete facing of the surface.

At the end of the cycle, the tool rapids to StartHgt, then rapids back to the start position. Refer to Figure 5-10.

Figure 5-10, Face Cycle Tool Approach

To program a Facing cycle:

1. In Edit Mode, press Pocket (F4) to display a pop-up menu.

2. Move the highlight to select Face, and press

ENTER to display the

FACE POCKET Graphic Menu. Refer to Figure 5-11.

Figure 5-11, FACE POCKET Graphic Menu

CNC Programming and Operations Manual

P/N 70000504I - Programming Canned Cycles, Ellipses, and Spirals

NOTE: ZDepth must be lower than StartHgt. StartHgt is 0.100 inches

(2.0 mm) above the work surface.

FACE POCKET entry fields:

ZDepth Absolute depth of the finished surface. (Required) StartHgt Absolute Z position the CNC rapids to before

feeding into work. (Required)

XStart X coordinate of the starting point. (Optional) YStart Y coordinate of the starting point. (Optional)

NOTE: Enter the required absolute XStart and YStart coordinates

when possible.

Length X-axis length to be faced. (Required) Width Y-axis length to be faced. (Required) XStepover Width of cut in the X-axis direction. When no value

is entered, the CNC defaults to 70% of the active tool radius. Maximum step-over permitted is 70% of the active tool radius.

YStepover Width of cut in the Y-axis direction. When no value

is entered, the CNC defaults to 70% of the active tool radius. Maximum step-over permitted is 70% of the active tool radius.

NOTE: Enter either an X or Y step-over. Do not enter both. NOTE: The Program Editor inadvertently will allow you to write a

block containing a Stepover value greater than 70% of the active tool radius. To reveal this type of error, test the program in the Draw Graphics Mode.

Tool# Active tool. (Optional)

3. Enter the required values and settings in the entry fields.

anilam 3000 User Manual

Specifications and Main Features

Frequently Asked Questions

User Manual

Section 1 - CNC Programming Concepts

Programs

Axis Descriptions

X Axis

Y Axis

Z Axis

Defining Positions

Polar Coordinates

Absolute Positioning

Incremental Positioning

Tool-Length Offsets

Tool Diameter Compensation

Using Tool Diameter Compensation and Length Offsets with Ball-End Mills

Angle Measurement

Corner Rounding

Line-to-Line Corner Rounding

Line-to-Arc Corner Rounding

Arc-to-Arc Corner Rounding

Chamfering

Plane Selection

Arc Direction

Section 2 - CNC Console and Software Basics

Console

Keypad

Programming Hot Keys

Label or Name Key Face Purpose X

Label or Name Key Face Purpose

Editing Keys

Label or Name Key Face Purpose

Manual Operation Keys

C L E A R

Operator Keys

SPINDLE OFF

Label or Name Key Face Purpose

E-STOP

Soft Keys (F1) to (F10)

Off-line Keyboard (Optional)

Software Basics

Pop-up Menus

Screen Saver

Switching Selections with the Toggle Key

Clear Key

Operator Prompts

ASCII Chart

Cursor and Highlight Functions

Entering Text

Typing Over and Inserting Letters and Numbers

Deleting Characters

Messages/Error Messages

Section 3 - Manual Operation and Machine Setup

Powering On the CNC

Shutting Down the CNC

Emergency Stop (E-STOP)

Performing an Emergency Stop

Activating/Resetting the Servos

(Re-)Starting the Spindle

Manual Mode Screen

Primary Display Area Labels

Secondary Display Area Labels

Position Display

Manual Machine Operation

Manual Mode

Auto Mode

Mode Settings

Activating Manual Mode Rapid or Feed

Setting a Feedrate

Adjusting Rapid Move Speed

Overriding the Programmed Spindle RPM

Absolute/Incremental Modes

Inch/MM Modes

Setting Absolute Zero

Defining Absolute Zero in X and Y Axes

Presetting the X- or Y-Axis

Fixture Offsets (Work Coordinate System)

Setting Tool Change Position

Locating Tool #0, Z0